[rolloblues]

Hi all, I'm developing a model of a regenerative chamber for glass furnace.
I'm using a porous model for the refractory honeycomb structure responsible for the heat recovery.
I correctly defined the solid phase for the porous media.
I'm using a non equilibrium model for heat transfer inside the porous media and I'd like to assign a linear dependency for the solid temperature as a function of vertical coordinate.

In CFX-Pre 14 I figured out how to define a heat source for the solid phase but nothing about a temperature function. The only thing I can do is keep the solid phase as "isothermal" at a fixed temperature which clearly is useless for me.

Does anynone knows a workaround (maybe with UDF or something) to assign a temperature profile to the solid phase in the porous domain?

What is puzzling me is that you can actually do this in the initialization tab for the porous domain but of course it won't be a stable condition for the calculation.

Thanks in advance

[Opaque]

I am not certain what you are trying to achieve by using the porous media non-equilibrium model this way.

Imposing a fixed temperature profile in the solid material of the porous media, as well as the heat transfer coefficient is equivalent to introducing a energy source term in the fluid phase equal to +/- HTC * (Tsolid - Tfluid). The non-equilibrium approach will not add any benefit to your model if that is the what you are really trying to do.

[rolloblues]

Originally Posted by Opaque

I am not certain what you are trying to achieve by using the porous media non-equilibrium model this way.

Imposing a fixed temperature profile in the solid material of the porous media, as well as the heat transfer coefficient is equivalent to introducing a energy source term in the fluid phase equal to +/- HTC * (Tsolid - Tfluid). The non-equilibrium approach will not add any benefit to your model if that is the what you are really trying to do.

No I can't use a source term for this reson:
I have two fluids flowing through the porous domain.
Lets say Fluid1 initial temperature is 300K while Fluid2 is 800K.

If I define a heat source inside the porous domain (W/m^3) this is a fixed value for all fluids. Each fluid receive locally the same amount of heat.

This is incorrect because as the solid temperature is a fixed value (in the real world) Fluid1 should receive more heat from the solid phase than Fluid2 which is hotter.

(Tsolid-Tfluid) is different for each fluid but a simple heat source won't take it into account

[Opaque]

My advice is to check some of the tutorials, and the theory of how sources are setup in ANSYS CFX. For multiphase cases, you must also read about BULK SOURCES.

Based on your description of the problem so far, a sample CCL for a multi fluid domain source to be applied to all fluids in the domain

FLOW: Flow Analysis 1
DOMAIN: Domain 1
    SUBDOMAIN: MySource
      Coord Frame = Coord 0
      Location = MySourceMesh
      BULK SOURCES: 
        Option = Use Volume Fraction <<<<<< Account for the volume fraction of the fluid
        EQUATION SOURCE: energy
          Multiply by Porosity = On <<< Your choice based on what net effect you want
          Option = Source
          Source = htc * (Tsolid - Temperature) <<< Different values for each fluid since Temperature is taken for the fluid equation being solved.
          Source Coefficient = -htc <<< Linearization coefficient
        END
      END
    END
END
END

Hope the above helps,

[rolloblues]

Very interesting...I didn't know that it's possible to use "temperature" in a CCL without specifyng the fluid (If more than one is present). I'll give it a try...

Thank you very much!

[rolloblues]

I did exactly what you suggested me but didn't work.
(Tfluid1-Tfluid2) at the bottom of the chamber is 600°C while at the top is 400°C.
I expect to find a smaller gap (50° approx) at the top.

Any Ideas?

[Opaque]

Without having the case details (geometry, mesh and physics setup), it is very difficult to advice via the forum when it comes down to expected/unexpected results.

As you have probably already read in the forum, it is always good to start with a simplified version of the problem, and ramp up the complexity to get a better understanding of what may be introducing a problem.

Have you tried to modify the porous media tutorial (catalytic converter) ? Selecting the geometry of a tutorial, and making incremental changes to reproduce your problem allows others to pitch in since you only have to exchange the CCL setup.

[rolloblues]

You're absolutely right but you see: I already succesfully set up the same model with just one fluid flowing through the porous domain. Problems arose when I added a second fluid. Form that moment I still haven't figure out how to deal properly with a multicomponent heat transfer in the porous media