Hi,

I'm now facing a big problem with fluent. I have to model a high temperature device wich comprises a porous media and a high temperature fluid zone. The problem is that by default a porous zone is considered as a fluid zone for the radiation and the radiation can pass trough the porous medium. It's not possible to consider that one side of an internal face participate to radiation and the other doesn't since it makes a bug during the computation and I can't define this interface as a wall since it will block the flow. There is also a problem using UDF since a UDF for special radaition can't be attached to any boudary condition exept a wall. Do you see a way to overpass this problem, or is it impossible. Thank you Pierre-Louis Schmitt

Hello Pierre-Louis Schmitt,

I work in research and development of volumetric solar receivers. You are facing a problem which is also highly relevant for me. In fact, I tried to get answers from Fluent in these regards for a very long time (few years), but they never answered it satisfactorily.

In the past we have used another commercial CFD package and augmented it with a lot of user coding to treat radiation in a participating medium, inter-surface radiation, porous medium treatment for HT and resistance to flow, chemical kinetics and more. In these models, it was assumed that in the volume occupied by the porous medium two distinct temperatures prevail - one for the fluid and the other for the solid. It was also assumed that the fluid is non-participating in the radiation (which is usually a good approximation), and that the porous medium is represented by its equivalent effective radiative properties. The relevant temperature for this medium emission, according the the above assumptions, is the solid temperature of each cell. This model worked fine as long as the other CFD package (no names mentioned...) did not fail. However it failed whenever the geometry was not trivial and in many other cases related to the problem physics, so we had to abandon it.

As far as I understand, there is no straightforward treatment of something similar in Fluent, as it assumes a SINGLE temperature in a cell, which is the FLUID temperature in the case of a porous medium. As this choice is limited and inappropriate to our needs (and probably to any body's dealing with radiation in a porous medium) it seems to call for a massive UDF coding. Being relatively novice in Fluent, I have not started it yet, and it may take a long time to get there.

As I started, I hoped this will be solved by Fluent, but they don't seem to tend to do it and/or did not understand the need for it.

Sorry I am not helping you here, just sharing my point of view. Maybe someone else (a more experienced user, and hopefully some expert from Fluent support or development teams) will have a constructive solution (or say what I claim is wrong, and this is already solved...).

Rami

Unfortunately, it seems nobody responds. It is regretful that Fluent employees are not responding either... Let's hope someone will soon.

Pierre-Louis Schmitt,

Did you get any response/help on this issue? I would be very grateful if you can share with me and this forum.

Thanks, Rami

Unfortunately I didn't get any response on this problem, I found a kind of "technic" to overpass the problem for simple cases. on a first step you compute a solution considering the porous zone as a solid zone with a thermal conduction equivalent to that of the porous medium, fluid zone is kept normally. Then you print the profile of temperature, reload the case with the porous zone and then impose the profile of temperature on fluid zones.

I think this hypothesis is good when the velocity of the flow in the porous media is low. It's the only way I found to get a simulation of my device.

Pierre-Louis Schmitt

Thank you. This workaround may be useful in your case, but not in more general like mine. Hopefully someone (FLUENT stuff, please respond!) will suggest a comprehensive solution, since the need to consider porous media participating in radiation is quite common in many applications.

[Rami]

Originally Posted by Schmitt pierre-Louis
;151747

Unfortunately I didn't get any response on this problem, I found a kind of "technic" to overpass the problem for simple cases. on a first step you compute a solution considering the porous zone as a solid zone with a thermal conduction equivalent to that of the porous medium, fluid zone is kept normally. Then you print the profile of temperature, reload the case with the porous zone and then impose the profile of temperature on fluid zones.

I think this hypothesis is good when the velocity of the flow in the porous media is low. It's the only way I found to get a simulation of my device.

Pierre-Louis Schmitt

I am still trying to have FLUENT development/support constructive response to this issue. As of now, they seem to treat this as a low priority issue in the development, since they consider this as something of little interest to other users and/or merely academic problem.

Are there any others (except me and Pierre-Louis Schmitt) who need this combination of radiative heat transfer in porous media and suffer from this apparent FLUENT deficiency to its treatment?

[Rami]

I have just noted this issue was already discussed for a long time. Here is one thread, dated 2001:
http://www.cfd-online.com/Forums/flu...ous-media.html

So it seems that there is interest in radiative HT in porous media. Any others interested, so we may convince FLUENT to finally do it right?

[Rami]

No one? Am I the only one in need for such features?

[waltastisch]

No you're not alone with this problem. I face the same problem in a high temperature furnace in which a porous body is sintered. It still seems impossible to have radiative heat transfer to the porous zone as well as fluid flow between the porous zone and its surroundings in FLUENT

[Rami]

It's funny. I have already gave up using Fluent for these kind of problems. Recently, a visiting student at our group has told me he had received a UDF for this kind of problems from Fluent (after long discussions with them). It is called "dual cell method", used in a tutorial called "Light-Off simulation for Catalytic Converter" dated April 1, 2005 by Fluent Inc., and in principle uses a (very inefficient and not elegant) method, in which the mesh is doubled, part for the solid and part for the fluid, and the UDF couples both to enable treating radiation (if I correctly understood). I did not check it myself - since we no longer hold a Fluent license, as it seemed inadequate for our needs - but was told it does the trick (though inefficiently). I just wonder why the Fluent guys did not suggest it to me when it was rellevant...

Maybe you can ask them about it, having all the details above.

[waltastisch]

I was offered this UDF as well, but since we have rather large and complex models, we decided that this is not the right choice.

To our luck, our problem is thermally uncoupled. The gas flow and the reactions within the porous medium are locally chemically important, but of neglible impact to the global temperature or flow field. Therefore we calculate the problem twice with the same model: first time the porous zone is just a solid, thermal radiation is calculated OK this way. The second time we calculate the same problem again, but the temperatures are taken as fixed values from the first run. Therefore radiation does not need to be solved and the porous medium formulation of FLUENT can be used.

This seems all quite OK for our special problem setup, but it is still strange that FLUENT does not provide a standard method to handle this...

[Rami]

Hi Walter,

Out of curiosity: where are you working and what are you specializing in (if you wish to tell, of course)?

The reason I am asking is also due to the fact that we tried very hard to get a solution for our problem (a volumetric solar receiver) with Fluent. This was after we had developed all the required capabilities (radiation and chemical kinetics in a general porous medium) for another package (PHOENICS), but had a lot of problems with PHOENICS itself (mainly lack of generality in the geometry and grid and too many bugs). It took ages to get replies from Fluent, and they never mentioned this dual cell UDF, and in general - seemed like doing us a favor answering at all. I suspect it was since we are in academia, holding a single seat academic license. Your answer may help support my suspicion.

At the moment we are looking again for a suitable package, and I think we will give Fluent another shot, but will also try others, with the hope to get more collaborative and constructive attitude.

Rami

[waltastisch]

Hi Rani

We're commercial users (only single license) and we use our models to calculate global models of high temperature furnaces. Within the oven we have porous solids which show some slow chemical reactions with the oven gas - we didnt' care about these reactions up to now. We want to extend our oven models to see the evolution of these chemical reactions as well. At the current stage we're just planning these steps. It'll take some months to do the programming and see how it works. I'm rather confident we will be able to do it in the way mentioned. To me, the Fluent support seems sometimes a bit slow and sometimes you have to remind them to take care of the question - but its generally OK.

[pilou]

Hi, I finally found a way to overpass this problem

I made a UDF that I copy past here :

DEFINE_PROPERTY(abs_coeff,c,t)
{
#if RP_HOST
real abs;

{
if (THREAD_ID(t) == valeur1)
abs = absp;
else
abs = 0.5;
}

return abs;

#endif

}

This UDF basically attach a different coefficient on the different zones depending on the zone ID. This way, the radiation in the porous medium is not perfectly equal to 0 but is very low and it gives a good approximation of the porous medium behaviour regarding the radiation.

This UDF is ready to be used in parallel processing.
Hope it can help

Pierre-Louis Schmitt (Pilou)

[oky]

Hi everyone,

I'm trying simulation porous media in rectangular channel, but the result isn't suitable with any research.

So, would you help me. I wish someone can check my simulation and give some reports if there is something wrong.

Thank you for your help.
Please send your e-mail, than i will send you my works to to your email.
my email: oky.andytya.net@gmail.com

Regrads,
OKY Andytya P

note:
I use ANSYS Fluent 6.3 [CFD]

[pilou]

Can you give us a few more information about your problem, type of porous medium, are you using a radiation model, what are the values of viscous and inertial resistances you are using...
Maybe we can help without the .cas file.

Regards

[mystic_cfd]

i am also one of the disappointed users of Fluent with regards to porous zone modeling.

if you still have to decide on a code, have look at CFX. In the latest release (13), they claim the following:
"In ANSYS CFX technology, porous CHT objects can now be modeled with separate fluid and solid temperatures. A user can specify the interfacial area density between solid and fluid together with a heat transfer coefficient. Energy is then conducted through the solid based on the solid properties and exchanged with the fluid."

Since CFX and Fluent are set to merge, we only have to wait another 3 or 4 years to have it in Fluent as well...

[oky]

For anyone, especially Mr. Pilou

Thank you for helping, i'm a student. I want get the flow and heat transfer characteristic in porous medium.

I have a channel with two baffles porous medium.
From the bottom of channel, i give heater.
The porosity is 15%.
No Radiation.
I'm trying to simulation in Laminar and Turbulent condition.

[Hìr0]

Originally Posted by pilou

Hi, I finally found a way to overpass this problem

I made a UDF that I copy past here :

DEFINE_PROPERTY(abs_coeff,c,t)
{
#if RP_HOST
real abs;

{
if (THREAD_ID(t) == valeur1)
abs = absp;
else
abs = 0.5;
}

return abs;

#endif

}

This UDF basically attach a different coefficient on the different zones depending on the zone ID. This way, the radiation in the porous medium is not perfectly equal to 0 but is very low and it gives a good approximation of the porous medium behaviour regarding the radiation.

This UDF is ready to be used in parallel processing.
Hope it can help

Pierre-Louis Schmitt (Pilou)

Hi Pilou, can you clarify why you want low absorption coefficient in the porous medium, please? I have the same problem simulating a flow passes through the stainless steel. By default partecipates in radiation is turned on for the porous zone and I know it is considered as a fluid zone. If I want the porous medium radiates as well as the wall of the furnace I think I have to increase the absorption of the porous zone to simulate the increase in heat transfert between fluid and solid due to the radiative contribution. I set high absorption in the SS material properties but the contour of absorption shows only the fluid absorption. Is there a way to pass to fluent the abs_eff as done for k_eff. The same for emissivity of the porous solid.

Another question....how can you set the emissivity of the fluid? I can find any option.

Thank you so much! Let me know, please!

Luigi