How to treat the jumpperiodic boundaries with the fluent!please help me!
Hello,everyone!
How to treat the JumpPeriodic boundary contions in the solution of solid and fluid thermal coupled problems in order to gain the effective conducitivity under the condition where there is no flow exist in the computational domain. Since the filesize of this pape exceeds the limit of the forum, i can not upload the paper that i read.So just a URL is presented for you ,and i am very sorry for that. Please help me,everyone!! Tell me how to carry out this Special boundary condition with fluent? Because no flow exist in the domain,the wall boudary condition is coupled wall, for the steady state,how to impose a temperature drop on the heat flow direction,i.e how to impose a temperature gradient on the periodic faces? The paper i mentioned, which you can see using the URL,had presented the method and the discreted equation sets.But i can not understand how to do the same work using the method, since a similar problem is under accounted for me. please,help me!!thanks everyone!! URL:http://asmedl.org/getabs/servlet/GetabsServlet?prog=normal&id=ASMECP0020044711Xa000 247000001&idtype=cvips&gifs=yes Title:A Numerical Technique for Computing Effective Thermal Conductivity of FluidParticle:confused: 
Can't access the paper as it's from a conference proceeding and requires a purchase but I managed to find the paper myself through my own database. I skimmed through it, so my interpretations may be immature, if I am wrong on anything, someone please correct me.
I disagree with the author's calling it the equivalent of the constant heat flux periodic condition since that is not how the constant heat flux case is treated in Fluent and many other software/schemes. In these software, the jump discontinuity in the bulk temperature is not applied, rather the bulk temperature remains constant by solving the temperature gradient separately (because the heat flux is known). This difference will may the simulation difficult or maybe impossible in Fluent. Even more so, the authors specified a temperature gradient which is inconsistent. How can you specify a constant heat flux and also the temperature gradient? To get the periodic heat transfer with no flow simply setup your case. Initialize the flow with 0 velocity everywhere. And disable the computation of the momentum equations (flow). Then the solver will only solve the energy equations. There may be some numerical errors associated with assigning a 0 velocity everywhere, since numerically 0 is just a very small number. Hence your results may be accrue some inaccuracies. You can use any viscous model since you are going to disable it anyway. But I suggest using a laminar model so that the turbulence modelling parameters don't add any more errors. Unfortunately, if you enter a mass flow rate of 0 in Fluent, this may cause the bulk temperature gradient to blow up. The temperature gradient is calculated by dividing the total heat addition by the incoming heat capacity which is now 0. The other problem is the constant bulk temperature. You won't have any conduction through your embedded solids since there is no temperature difference in the flow. Additioanlly since there is no flow, there is no net direction of heat transfer and no direction can be assumed for the temperature gradient. This is a conceptual mistake I believe on the authors part. I am not completely familiar with this topic so I will suggest by asking questions. Does this problem require the use of periodic conditions? Can you not simply specify the fluid temperature at the inlet and exit (by making them static walls) and then solving the same problem? This is basically what the authors did by specifying a temperature gradient. 
Treatment of jumpperiodic boundary with the fluent
Thanks,LuckyTran.
I am grateful for your help,and appreciate any information that you give me,especially for that you had download the paper and had a careful reading. As we study the porous media on the microscopic scale(cell or representive element volume),which is a basic unit ,in order to replace the object of the whole block material, a REV may be choosed to reduce the computation expense.So the periodic boundary condition may be more appropiate in this case.Just as you said,the same obfuscation is for me when i managed to solve the problem with the fluent. Yes,you are right.The suggestion that setting the inlet and exit with the wall boundary condition ,rather than periodic boudary condition,may be a good idear.I will try it as you said. At last, the paper that using the fluent solve this problem will presented for you,please tell me how to interprete the meaning of that "Computations are performed using a modified version of the commercial code FLUENT(page 796)",at your convinience. Title:Direct Simulation of Transport in OpenCell Metal Foam. Author: Shankar Krishnan et. Journal:Journal of Heat Transfer URL:http://asmedl.org/getabs/servlet/GetabsServlet?prog=normal&id=JHTRAO000128000008000 793000001&idtype=cvips&gifs=yes My email :chenzhana@163.com Also,you can have this paper by message. Very,Very Thanks for your help. Have a nice day,My friend.Good luck. 
Quote:
It might be of importance to note that, although the bulk temperature is maintained constant for the constant heat flux case, the periodic jump condition is applied for the constant wall temperature case. I double checked and no changes were made to Fluent since version 6.0 so there is no way that the authors could've used the specified heat flux condition as that would have resulted in a constant bulk temperature which contradicts many points they made. I'm not sure what's going on here. I understand the argument for periodic geometry but am not sure how that is applicable. Since we all agree that the temperature gradient is arbitrary anyway and no bulk fluid motion exists, so even setting the wall temperature is equivalent to a periodic heat transfer (if periodic heat transfer is even applicable, which it really isn't). I do however see how it is possibly doable by tricking Fluent into solving it (since you can input a direction vector so that Fluent can assume the flow is in a certain direction). A huge problem I imagine that would be encountered with Fluent is the spatial discretization scheme (which is either 1st or 2nd order upwind). For a stagnant flow there is no upwind cell (because there is no advection). There is a corresponding upwind cell in the heat diffusion sense, but that is not what Fluent is looking for when checking the upwind condition (it is looking for face velocities). 
Treatment of jumpperiodic boundary with the fluent
Thanks,Lucky Tran.
if this question could not be solved by the software fluent ,can you give me some suggestion on other software,as i am tenderfoot. I means that if there are some other open codes (free software,like openfoam),through making any modification by myself,can solve this problem,because i have another problem like this,which is about the mass transfer. (species i mass diffusion flux enter the domain from the top boundary) http://asmedl.org/getabs/servlet/GetabsServlet?prog=normal&id=ASMECP0020044711Xa000 365000001&idtype=cvips&gifs=yes (species i mass diffusion flux enter the domain from the down boundary) In order to simulation the situation of the full development, i manage to use the periodic boudary to solve this problem.But you know,in the fluent,its capability to solve the heat transfer and flow with some geometry repetition. So if i want to solve it,what need i do ? It is just the similar,and like this problem also present some other reasurech field.There are some common character that the upstream field informations were not known which need to impose the downstream(right side)informations on the upstream(left side),and continuously iterate until the difference between the upstream and downsteam keep a constant. Thus how to treat these problems ? Fluent can do? Thanks a lot,my friend! My english is poor,if some mistakes happened in the text,please tell me ! Thanks again!!! Title:MACROSCOPIC MODELING OF TURBULENT MASS TRANSPORT IN HETEROGENEOUS POROUS MEDIA 
For the case of no mass diffusion, it should still be treatable by taking the fluid to be a solid.
However, there should not be confusion between periodic geometry and periodic heat transfer. Sure I accept that the geometry is periodic but there is no need for the resulting heat transfer problem to also be periodic. Periodic heat transfer leads to very unstable results. So instead, I would apply an arbitrary temperature gradient which is what the aforementioned papers did anyway. Also, no use of periodic boundary conditions need even be applied since they don't matter. The physical geometry is probably periodic, but the numerical simulation does not care as long as it has the proper boundary conditions (which we agree a simple temperature gradient will suffice). Mass flux is not a periodic flow, so you must abandon the periodic approach! But I do not think that is much different than what you are attempting, since periodic bcs are not needed anyway. 
Jumpperiodic boundary
Thanks,Lucky Tran.
Yes,you are right, i agree with your opinion,especially on the species mass fraction.As we know, the conservation of mass,moment and energy.If the species l enter into the domain from any boundary ,that will cause the velocity field changing.The inlet and outlet could not keep the same profile whether the fluid is a compressible one or not.Simutaneously,the mass variation will also cause the moment and energy changing. Thanks very much again. Take my best wishes to your family.Good luck!! your friend:Chen Zhan 
Dear Lucky Tran,
I found your knowledge about periodic flows pretty impressive. I am simulating a pipe with solid modeled and defined its inlet and outlet as periodic. In postprocessing, I need to find the temperature at inlet and outlet and take the mean. But since I had taken only the bulk temp at periodic condtion dialogue box,, I am unaware that how to take the mean? Please hlep me that I do not understand the philosophy of temperature gradient in case of periodic condition. How I get temperature at outlet that does not exist anymore? 
by the way I have flux on top wall. I mean I have top wall then solid part, then interface and then fluid region

Quote:

Dear Lucky,
Thanks a lot. 1. Since my inlet and outlet has been utilized in creating periodic boundary, how can I suppose to take energy balance. I have only one surface now, that is periodic. 2. What is the general method for seeing energy balance. I mean that energy equation residuals also indicate that. For mass flow, we can say that inlet and outlet must be equal, what about energy? Please elaborate your respective opinion. 
1. You still specify an inlet bulk temperature through the periodic boundary conditions menu. Hence you know inlet temperature. You know the heat flux (it's a specified boundary condition). You should know, or at least can determine, the surface area through which the heat flux acts. Hence you can calculate the total heat added/removed (heat flux * surface area). With this you can calculate the exit temperature via an energy balance. Of course you are assuming that the solution obtained via Fluent satisfies this energy balance (which it should if everything is behaving as it should).
2. After you make a boundary periodic the boundaries are hidden. You can define a surface beforehand so that you can still compute the exit temperature after. You might have to be a little creative. I think you can get the temperature rise using rpgetvar but I don't know how at the moment. 
Quote:
I tried to use pressure gradient method in periodic boundary but there is a monitor for its convrgence in Monitor> statistics. That shows for Pressure gradient convergence. It takes very very long to converge however, using normal inlet and outlet (without interfaces) conveged the solution in less than 3000 iterations. here it is taking more than 50000 and still not converge. Question How to see convegence in case of periodic translation flow? 
All times are GMT 4. The time now is 21:17. 