[pprtyy]

Hej,

your comments are good. But CFX might be a solution, since it has the function to analysis conjunction of fluid and solid in porous material

[fredom]

Hello everybody,

I am interested for this topic, because I would like to simulate heat transfer between hot wall 1 (473K) to wall 2 which is perforated sheet. The distance between them is 200mm.

The purpose is to define the temperature of the perforated sheet. As the velocity inlet is low 2m/s and it pass paralle to the perforated sheet, should I define the perforated sheet as a porous jump ?

Thanks very much for your comments..

Fredom

[Fluent_user_2015]

Hello everybody,

i am facing the same problem as described above. in want to simulate combustion iside a porouse zone in fluent. Radiation is also very important in my case. Even in the newes version of fluent (16) it seems not to be possible to consider radiation from porous media in porous zones.

Has anybody a solution for this problem?

Thanks very much for your help!

[Rami]

Dear Fluent_user_2015,



I recently joined another group (hydrology research) and do not use Fluent any more, nor radiation and thermal issues in general. However, I' try to help.


Please find below the (long) correspondence I had with Fluent support that addresses using radiation solvers with thermal non-equilibrium in porous medium. I hope it is helpful.


The trick is described in the 29/01/15 message from SKS:
(rpsetvar 'rad/enable-netm? #t)
and further discussed in following messages. You have plenty of information and I trust it should suffice.

Best luck,

Rami

From: Rami
Sent: Thursday, February 06, 2014 14:42
To: 'SKS'
Subject: RE: SR Owner Notification SR#: ---has been updated

Hi SKS,
This is what I suspected…
Thank you for your efforts,
Rami

From: SKS
Sent: Thursday, February 06, 2014 14:19
To: Rami
Subject: Re: SR Owner Notification SR#: ---has been updated

Hi Rami,

I can reproduce the problem. I had a discussion with Development and found that currently P1 radiation with NETM will not account for solid!!. So, I would recommend, if you want to use P1 radiation, please use the UDF you developed. You may use in-built DO radiation with NETM, as programming DO radiation is not an easy task. Since development is creating compatibility with one radiation model after another, it will take some time for them to make it fully available. Please bare with us.

Thanks
SKS

On Thu, Feb 6, 2014 at 4:25 PM, Rami wrote:
Hi SKS,
The files of my Feb 4 2014 message are attached again. It would be nice (and less error prone!) if it can run using the same UDF, input files (cas and inp.txt) and settings (except P1 or DOM models).

I am grateful for your dedication!

Rami

From: SKS
Sent: Thursday, February 06, 2014 12:47
To: Rami
Subject: Re: SR Owner Notification SR#: ---has been updated
Hi Rami,
Sorry that initially I understood your question very differently. That is the reason my answer did not make sense now.
Now, I tried to run the case file you sent me on Feb 4 2014, I am not able to initialize the case. It seems that the case file is corrupted. Could you please check and re-upload the files?.
By the way, you did not do anything wrong. This kind of problem occurs when it is in the development stage. As FLUENT is getting bigger and bigger, we need to make sure that any piece of new code must work with all combinations and we must validate it. Once I get the correct case file, I will investigate and let you know the workaround if there is any
Thanks
SKS

On Thu, Feb 6, 2014 at 2:48 PM, Rami wrote:
Hi SKS,
Thank you for answering, but this time I do not understand your reply.
As you may see in the files I had sent you on Feb 4, 2014,
·I had enabled NETM + radiation before setting up the case.
·The NETM option was used and created the solid zone.
·I had enabled radiation in the solid zone (and also in the fluid, with fully transparent properties).
·I initially chose DOM for radiation.
·I prescribed BCs (specifically, collimated radiation using the Qirr DEFINE_PROFILE macro from the on the front surface, inlet:012)
·It all ran fine.
·I then only changed the radiation model from DOM to P1 (without any other change in the case file and in the udf), and then the radiation properties disappeared from the solid material (foam), and the radiation BC settings disappeared from all solid surfaces.
Is there anything I did wrong?

Thanks,

Rami

From: SKS
Sent: Thursday, February 06, 2014 04:40
To: Rami
Subject: Re: SR Owner Notification SR#: ---has been updated
Hi Rami,
Did you enable Participation of radiation for solid in cell-zone condition panel?
Since NETM + Radiation is in the process of development, I would recommend you to use the UDF which is specifically written for your purpose, only if enabling "Participation of Radiation" did not help. NETM + Radiation feature will be available only after the compatibility check with all other models and the accuracy of the code is tested extensively. Hopefully, it will be available in R16.
Thanks
SKS
On Tue, Feb 4, 2014 at 7:31 PM, Rami wrote:
Dear SKS,
Thank you so much for your wonderful and prompt help! Everything worked as you suggested.
Now, I still wish to use the built-in P1 model with the scheme command trick to allow using it with a non-equilibrium thermal model (NETM) in order to compare it to experiment described in Sec. 4.2 and Figs. 10-11 of the original reference paper (attached again for your convenience). I imagined that with the new UDF, cas and input files (attached) I need to only switch between the DOM and P1 and that’s it. However, it seems that the solid has neither access to the absorption and scattering coefficients nor to the BCs (the Marshak BCs at walls and possibly the collimated irradiation in the front).
I tried also (in the attached cas file) to put the absorption and scattering coefficients of the solid in the fluid material slots, but the temperature is almost uniform, since the irradiation is absent.
Is there a way to do it, or should I stick with the former udf, modified from the UDF Guide example?
BTW, I have found that I may read the input file in a DEFINE_INIT rather than DEFINE_ON_DEMAND, which is more convenient.

Thanks a lot for all you did thus far and also in advance!

Rami

From: SKS
Sent: Tuesday, February 04, 2014 11:49
To: Rami
Subject: Re: SR Owner Notification SR#: ---has been updated
Hi Rami,
Glad to know that you are happy with the scheme command though it has some issues.
Yes. This kind of problem is expected, as this feature is not fully developed. That’s why I mentioned in my last mail that, this has not been tested extensively. This is the same reason why this feature has been hidden. We provide the scheme command as a workaround for the users who explicitly ask for the combining of NETM and radiation. Developers are working to make this feature available to all users (without the scheme command). It may be available at R16. In R15 we do not have any option. So, please follow the same order to setup the problem.
1. As a workaround for the error, when you try to replace the mesh switch to equilibrium thermal model -> replace mesh -> enable NETM. This will avoid the error. But, this is just a work around. When this model is available in later version, you will be able to use it in the same way you use for the other features. When you are using workbench you should change to equilibrium thermal model before you save the project. Please let me know, if this works
2. I looked at the UDF. It is better to use DEFINE_ON_DEMAND, as you are going to read the file only once in the whole simulation. The problem is that you are defined the variables are real. So, please convert the data types from real to float. It will read the data properly. I have tested it. It does read properly.
Thanks
SKS
On Mon, Feb 3, 2014 at 1:54 PM, Rami wrote:
Hi SKS,
I managed to use your suggestion and it seems to work fine with the DOM, but it is indeed tricky to use, and I have tweaked a lot to find the right order to set up a case using standalone FLUENT 15.0:
1.Start FLUENT.
2.Read the mesh file created by WB.
3.Issue the TUI command (rpsetvar 'rad/enable-netm? #t) .
4.Setup the case, including solving energy and DOM, then define the porous domain as non-equilibrium.
5.Add the UDF, build and load.
Doing it in a different order caused errors of various types, e.g.,
Error: received a fatal signal (Segmentation fault).
Error Object: #f
The case and the UDF files I used are attached.
Now I have two related questions:
1.Suppose I wish to replace the mesh with another mesh (e.g., to assess the grid independence), and the new mesh is, say, the attached FFF.msh . Just reading and replacing the existing case grid does not work, since the dual cell method was applied to enable the non-equilibrium porous zone. The new mesh zones and BCs are therefore yielding errors. How do I do it without having to go through the entire setting process again (with a good chance of missing part of the definitions)?
2.I would like to add reading input from a text file rather than putting them “hard-wired” in the UDF, but failed– all the parameters remained 0 (see the commented lines in the DEFINE_INIT macro within the UDF and the attached inp.txt as an example). The advice from my local agent (using a DEFINE_ON_DEMAND macro also failed). What have I done wrong?

Thank you in advance,

Rami

From: Rami
Sent: Wednesday, January 29, 2014 16:51
To: 'SKS'
Subject: RE: SR Owner Notification SR#: ---has been updated
Hi SKS,
I am still checking and have not fully set the case, but – it seems to work (with DOM)! I will let you know when I reach some conclusions.

Thank you so much!

Rami

From: SKS
Sent: Wednesday, January 29, 2014 13:07
To: Rami
Subject: Re: SR Owner Notification SR#: ---has been updated
Hi Rami,
I spoke internally as well as Radiation development manager and radiation team members. There is a rpvar to enable radiation model with Non-equilibrium thermal model. Before setup the case, type
(rpsetvar 'rad/enable-netm? #t)
in TUI. Then you will be able to enable Non-equilibrium thermal model with Radiation.
NOTE:

• It is available only in R15.0
• This has not been tested extensively. That is the reason, it is hidden.
• IMPORTANT: When you enable Non-equilibrium thermal model and close the cell-zone panel and reopen the same panel, you will notice that, FLUENT switches the Thermal Model to Equilibrium from Non-equilibrium. This is an artifact. I have reported this to development and they will fix this in R16. But, when you enable Non-equilibrium model and just click OK, solver consider Non-equilibrium thermal effect with Radiation. So, make sure that, each time you close cell-zone panel Non-equilibrium thermal effect is enabled.

Please let me know, how it went
Thanks
SKS
On Tue, Jan 28, 2014 at 3:09 PM, Rami wrote:
Hi SKS,
Thank you for your prompt reply! As I have already explained, the P1 is a severe compromise in the problems we wish to cope with, so I will prefer to use it only as the last line.
In the following I will add my response to each point you made.
If you would like to use FLUENT inbuilt Non-equilibrium thermal model and implement DO radiation through UDF, it is tricky. I am checking internally, if it has been done by anybody in ANSYS. I will get back to you, once I get reply.
Please check and let me know.
We can also try implementing energy equation for solid through UDS and use inbuilt radiation model. I haven't tested it or I cannot find any work done by anybody. But, by this way, you will be able to use DO radiation model without any problem.
This is unclear to me: I am having flow in a porous medium (foam), so I need to solve a fluid in a porous medium (mass equation, resistance terms and convection to the solid – all influenced by the porosity) + a solid energy equation (including radiation and convection terms). Please clarify how your suggestion copes with these while using a DOM for the radiation.
To answer your question regarding example in UDF manual, it should be Thread *t0 = THREAD_T0(thread);. Because, t0 is used as cell thread in later lines.
Being novice in C and writing UDFs, I tried your correction rather than mine in a case I ran, and got the same results. Thank you!

Best regards,

Rami

From: SKS
Sent: Monday, January 27, 2014 13:50
To: Rami
Subject: Fwd: SR Owner Notification SR#: ---has been updated
Hi Rami,
Great to know that you have implemented P1 radiation using UDF with the help of example in UDF manual!!.
If you would like to use FLUENT inbuilt Non-equilibrium thermal model and implement DO radiation through UDF, it is tricky. I am checking internally, if it has been done by anybody in ANSYS. I will get back to you, once I get reply.
We can also try implementing energy equation for solid through UDS and use inbuilt radiation model. I haven't tested it or I cannot find any work done by anybody. But, by this way, you will be able to use DO radiation model without any problem.
To answer your question regarding example in UDF manual, it should be Thread *t0 = THREAD_T0(thread);. Because, t0 is used as cell thread in later lines.
Thanks
SKS
/************************************************** *****************/

Technical Details:

Activity Description: I am actually looking for a better radiation solver (such as the DOM) rather than P1

Activity Detail: Dear SKS,

Thank you for your response. I am already aware of all you wrote, but this was not my query.

I need a better radiation solver to cope with the specular reflections and spectral effects of the quartz window. I was therefore asking if the P1 implementation example in the UDF guide (1) has a better option, i.e., is the limitation removed so that all the radiation solvers (especially the DOM) are already available in combination with the non-equilibrium porous media. I understand it is still not so (what a disappointment...).

I am already using a modified P1 UDF including all the details in the papers attached by Ed Moses on my behalf, but this is a very crude model, which does not allow for the spectral effect of the quartz (which is very strong, as it is nearly fully transparent below ~3.5um, and nearly black above it) and its specular reflections. The P1 model will also limit me in prescribing the incident solar irradiation to a more realistic case in which it is neither diffuse nor collimated. It is also known to be a crude and non-conservative approximation (also observed by Wu in the paper sent to you, both in the need to modify the BCs and in the comparison to the experiment).

If you can suggest a better approach than P1 (and not writing a full DOM UDF (2)... ) that overcomes these limitations, please let me know. I would be grateful if you could send it directly to Rami
Regards,
Rami

(1) PS: I suspect the P1 implementation example in the UDF guide has an error in DEFINE_PROFILE(p1_bc, thread, position), and the line "Thread *t0=thread-t0;" should be "Thread *t0=thread;" - is that correct?

(2) BTW, we had written a standalone DOM Fortran solver and implemented it in another CFD package long ago.

Thank you.

[User12]

Hello,

I am also trying to model radiation and porous media in fluent. Reading this thread helped me a lot to understand the limitiations of fluent regarding this matter.
My model is a sort of catalytic converter where the catalyst zone (porous media) is a metallic honeycomb at elevated temperature. Upstream this zone, the metal casing forms a really sharp cone, so this wall is very close and exposed to the front face of the porous catalyst and could get hot due to radiation from it. My objective is to model how much this casing is going to heat up. I am far from being an expert in radiation but, in my opinion, the front face of the porous media will behave as a solid surface in terms of radiation. Since fluent treats porous media as a fluid, I cannot define an emissivity for this face. Then, I tried to set a non-equilibrium thermal model in the porous media by following Rami's solution (previous post). Thus, a solid zone is created and the face emissivity can be defined. However, this wall appears as an external wall, or at least the boundary conditions that can be set are those corresponding to an external wall, i.e, heat flux with external emissivity, convection/radiation to a free media, and so on. I performed many tests and my conclusion is that the solid body is not interacting with its surroundings. Irrespective of the boundary conditions I try, the solution does not change. My impression is that this fictitious solid which is created is only connected to the corresponding fluid zone of the porous media in order to calculate the different temperature profiles (non-equilibrium in the porous media). Therefore, for my case, Rami's solution is not working. I spoke with fluent support but they cannot give me te solution for this problem.

Searching for an alternative, I built a very simple model in which I use DO and only solve for radiation equations. I found out that when I set a very high absorption coefficient in a gas zone, this behaves in a very similar way as a solid emitting at the same temperature, so maybe if I set a high absorption coefficient in my porous media, I could capture radiation of the front face as if it was solid. I was wondering if this trick could work out for my case, but I am not sure if I will negatively affect the model in other aspects. Can anybody advise on this? Does this make physical sense?

Thanks

[mmunige]

Dear all,

I am modelling heat transfer through a porous medium in fluent (from hot air to porous medium), have defined porous medium in fluid cell zone, resistance coefficients,
porosity, heat transfer coefficients since i am using non-equilibrium thermal model. this is transient 2D simulation. (a vertical column having porous material inside and top inlet for hot air and bottom outlet).

in start temperature distribution along the domain is fine and close to experimental values, but after 300 or 400 seconds temperature does not change or changes very little at all sections of domain and further it goes below the experimental values. I m using both fluid and solid properties as temperature dependent.
please guide me where i am doing wrong so I am not getting the uniform trend of temperature variation along the domain in whole simulation period.
please

Regards

[iam]

Dear Ramni,

Thanks a lot for posting your correspondence with Ansys support, it was really helpful to activate the non-thermal equilibrium option.

I am working at the moment in a surface burner which is conformed of a ceramic fibrous porous mat. How could I estimate the Interfacial area density, and the absorpion coefficient for the porous material?

Thanks a lot for your help!!