Can anybody suggest any paper or related book where heat transfer conjugate problem (conduction+convection) and its iteration process are treated with detail? Thanks

(1). The reason why you have this type of problem is because you are trying to solve two problems at the same time. (2). There are two ways to do: (a). formulate the problem as if it is one problem. In this way, you need to solve only one set of equations. (b). formulate two problems, one for convection region and one for conduction region. (3). In the first approach, you are going to have variable coefficients for convection terms, and conduction terms. And in the conduction region, the coefficients of the convection terms must be zero. (4). For the two region approach, normally the interface temperature is unknown, and can be used as a parameter. In this case, set initial guess of the interface temperature first. Solve the conduction problem, and solve the convection problem separately. You can then compute the heat flux at the interface, from both sides. Do this for a couple of cases with different interface temperatures. Then from these cases, you can come up with a simple interpolation, or extrapolation method to move the interface temperature. (5). Naturally, I am talking about solving the governing equations for fluid region, and solid region without any empirical data.

With your interpolating technique applied to one of point in the interface, it is possible to ensure that solid and fluid calculations are consistent in the interface (that is wall temperature and heat flux are equal in both sides). But what happen with the rest of the interface?. These conjugate problems are encountered for instance in internal cavities of aero-engines. You want that the solution is consistent not only at one point of the interface but in the whole cavity boundary. Is there any iterating process in order to approach the solution quickly? Papers or references will be appreciated. Thanks

(1). If the interface temperature is also non-uniform, then you need to update temperature each point. (2). The interface is similar to the interior points, except that you have different governing equations on both sides. (3). It would be easier to take the transient formulation approach. In this way, at any instant, you can predict the temperature at the next time step. (4). If you use heat transfer coefficient concept on the fluid side, then you can simplify the problem somewhat. But it is a semi-empirical approach, because the distribution of the heat transfer coefficient is normally unknown for complex geometry. (5). Conjugate heat transfer CFD simulation in turbomachinery is relatively new (last few years), you can take a look at the ASME/Journal of Turbomachinery and related ASME Journals in this area.

I have planned to use the heat transfer coefficient as a boundary condition for the coduction code. In fact, CFD calculation is done in order to obtain the correct boundary condition for the conduction solver. Calculating the heat transfer coefficient in the fluid side is not difficult at all and can be done first by performing a computation with adiabatic walls and then computing again with heat flux permitted accross the walls. The main obstacle is coming when enforcing temperature and heat flux equality in both sides all along the interface. The key point is to know how this updating and iteration process is done. Thanks for the hint

Peter, can you please elaborate on determining the fluid-side heat transfer coefficient from adiabatic and heat flux situations? How do you go about calculating h? Thanks.

Heat transfer coefficient can have arbitrary definitions depending on the temperature chosen as a reference value. One possible way of computing the heat transfer coefficient is to perform first a computation with adiabatic walls, this giving the adiabatic wall temperature which is used as a reference for the heat transfer coefficient. Then one has to compute two more cases: specifying the wall temperature at , say +/-100K the previously computed adiabatic wall temperature and permitting heat flux accross the wall. From these computations one can obtain two heat fluxes at two wall temperatures with the same reference temperature. Thus being possible to calculate the heat transfer coefficient all along the boundary with the equation: htc=(q1-q2)/(T1-T2). The reference value choice for the temperature is arbitrary, though in this forum has been recommended to use adiabatic wall temperature for compressible flow and free stream temperature for external incompressible flow. In internal heat transfer, it is possible to use the bulk or mean temperature.

Peter,

I have fooled around with this problem in my ASME paper FEDSM2001-18137. I did not mess with the heat trasfer coeff. at all. The iteration procedure starts by solving the fluid problem with a guess (nonconstant) interface temperature. Then, the heat flux is applied as a loading for the solid problem which returns the interface temperature and so on. The procedure does not converge in all cases - especially if the solid conductivity is low - but if it does, then the temperature and heat flux are continuous across the interface, witihin interpolation errors ofcourse. One nice feature of this approach is that the solid and fluid grids can be mismatched at the interface, which helped me out a lot.

The main problem is the long time for each iteration fo the fluid code - many hours for the fluid side and a few seconds on the solid side !

I hope this helps.

A. Suresh NASA Glenn Research Center

A.Suresh,

Many thanks for your message. The approach of solving this heat transfer problem depends on the tools that one has and their capabilities. I have read the ASME paper 2000-GT-282 where another analysis of this type is done. They are using an in-house FV code for the fluid-side and a commercial FE code for the solid-side. They explain some of the troubles that they found during the iterations and provide some recursive formula to minimize computational time. They also pay much attention on the different computing times of the two codes and recommend some actions: update the imput for one code enven before the other code computation is totally converged and others.

I will appreciate to take a look at your paper. I will give you an email address if you want to send it.

Thanks a lot.

(1). It seems to me that there are rooms for improvement in this area. (2). Conduction problem definitely will converge faster than the convection side. (3). As I said, it is a relatively new application field, and I think, a lot need to be done in the future.

A little late -sorry- but thanks.