# How is conjugate heat Transfer implemented in CFD codes?

 Register Blogs Members List Search Today's Posts Mark Forums Read

 April 29, 2020, 17:52 How is conjugate heat Transfer implemented in CFD codes? #1 New Member   Daniel Join Date: Aug 2017 Posts: 7 Rep Power: 8 Hello, Could could someone point me to a textbook or journal paper that describes how Conjugate Heat Transfer (CHT) is implemented in CFD codes? I am interesting in seeing what equations are implemented for the calculations of the heat transfer coefficients in CHT. Any help would be greatly appreciated. Thank you very much for your time!

 April 30, 2020, 07:31 #2 Senior Member   duri Join Date: May 2010 Posts: 245 Rep Power: 17 There is no special equations for CHT. CHT has solid element and fluid elements together. Both are solved with similar discretization. Temperature is the only unknown in solid and hence energy equation is solved with only thermal diffusion, source etc. Heat transfer coefficient is not solved or applied in this case. The fluid-solid interface flux and the face temperature is used to estimate the coefficient. Interface flux calculation from gradients differs with implementation style. userid42 likes this.

 April 30, 2020, 08:28 #3 Senior Member     Paolo Lampitella Join Date: Mar 2009 Location: Italy Posts: 2,169 Blog Entries: 29 Rep Power: 39 Well, it actually depends a lot from the implementation and the target code (I assume cell centered FV in the following), and no, there is probably no such thing around in the form of a book that I am aware of, so let me give my 2 cents. First of all, if by CHT we identify the heat transfer between a fluid and a solid region, you need to recognize that the boundary between the two is necessarily, from a coding perspective, an actual boundary for the fluid part. That is, you will still need pressure and velocity bc on the fluid side. It is the temperature that might seem to require no treatment, in the sense that solid-fluid boundary, if properly discretized, could work as any other interior face. But this is not anymore true if you need a temperature wall function, shell conduction, or a lot of other fancy treatments at the interface. For example, what happens if you have a CHT between two fluid zones, both with wall functions, and just shell conduction at the boundary? Thus, as a matter of fact, at least from the coding perspective, it makes a lot more sense to actually treat the solid-fluid boundary as a regular boundary and set up an internal mechanism to properly update the bc info in order for the regular bc to work also with a conjugate problem. So, the way you solve the problem is by iteratively coupling the fields on both sides of the interface. You can do it on a face by face basis (for each face you iterate until on both sides you converge) or during the global iterations (less robust of course, but less costly as well). What you need to do in such iterations is finding the wall temperature (or more than one if you have shell conduction) so that the heat fluxes on both sides (computed with the regular bc for given temperature) are equal. Iterations are necessary because, as soon as you have any non linearity, like a wall function, the problem can't be solved anymore analytically. As a matter of fact it might make sense to always do iterations (and you do only one if you have the analytical solution, that you might always use as initial guess). Let me also take the chance for trying to correct a misconcept that seems to be very common. In any serious CFD code the heat transfer coefficient can only be: - a post processing quantity derived from its constituents, which are all known in this case (including q) - an input for a boundary condition representing heat transfer toward an UNSOLVED and UNREPRESENTED fluid zone (e.g., you solve the flow inside a box and model the heat transfer with a fluid OUTSIDE the box using a heat transfer coefficient, as opposed with just, say, fixing the box temperature) So, to answer your question, with CHT implemented as explained above, you can just do your regular postprocessing because q is available at the interface as usual. The BC using the heat transfer coefficient, is just a regular BC, even with the shell conduction, and if you use it, it means you are not using the CHT in the first place. userid42 likes this.

 May 2, 2020, 00:59 #4 New Member   Daniel Join Date: Aug 2017 Posts: 7 Rep Power: 8 Thank you all for your prompt responses. Your answers are very clear!

 November 30, 2020, 10:48 #5 New Member   Vaibhav Join Date: Feb 2020 Posts: 5 Rep Power: 6 Hi Paolo, I am also formulating a code for CHT with coupled boundary condititons. The problem involves modeling the fluid domain with SIMPLE staggered gride for steady laminar flow and discretizing the diffusion equation for the solid domain. The problem is simply fluid flow between parallel plates with non zero thickness and constant heat flux applied to the parallel plates. (I am just trying to verify this conjugate model and use this further for developing model of heat pipes for my thesis). If I get nusselt number of 8.23, I can verify this code using that. I am getting issues with the coupled boundary conditions. The research papers I have been reading all suggest that I need to discretize the equations wrt time and use time steps to march through the solution. I wanted to ask if it is possible to achieve convergence using the steady state discretization? Also, I am employing the forward flux forward temperature back (FFTB) as well as the Temperature forward flux back(TFFB) methods which produces unrealistic results for this simple simulation for some reason. I have been trying to solve this problem for two weeks with no results. Any lead would be highly appreciated.

 December 2, 2020, 06:44 #6 Senior Member     Paolo Lampitella Join Date: Mar 2009 Location: Italy Posts: 2,169 Blog Entries: 29 Rep Power: 39 Let me first mention that I have no idea about any possible issue related to the staggered grid (probably none, but I don't know). Also, when I had to implement this, I already had too many complications to work on the ramifications of this or that algorithm. So, I worked with a full coupling on a face by face basis, as mentioned in my previous post. That approach basically implies solving many small 1d cht problems for each face center at the coupled boundary. The output of such problems are both T and q at the two sides of the face, which are the correct values given the current trmperature in the adjacent cells. What I found is that, with the local cht problem solved correctly, it has basically no relevance to the stability if you use the T or q on the two sides, nor if you do this with time step or iterations. Basically, I am using a fully explicit approach here, as temperatures from both sides of the 1d problems are the old ones, but I found it to simply work (yet, in the final system, there is still an implicit part wrt to adjacent cell, because everything is put down as a regular bc) So, unfortunately, I have no experience with other approaches. Indeed, I explicitly avoided them because I knew they might have stability issues