Conjugate Heat Transfer Simulation

The purpose of this project is to simulate the conjugate heat transfer in a pipe using Converge Studio. For this, an air flow is simulated through an aluminum pipe, which is receiveing a constant heat flux of 10,000 W/m2 at the outside wall. The objective is to understand the phenomena, run a grid dependence test and analyze the effect of the supercycle stage interval in the problem.

Geometry and Problem Setup.


The pipe has an inner radius of 15mm and 5 mm thickness. The length of the pipe is 200 mm, and the participating fluid is air (77% N2 and 23% O2), with an average kinematic viscosity of 1.562 e-5. Air flows in the positive z direction.

Case setup

The program will solve a transient case, using supercycling. The initial and final time are respectively 0 and 0.5s, and the turbulence model is RNG k-eps . Supercyling is a method typically employed in problems where there is an important difference in time scales, such as the heat transfer in solids and fluids. The heat capacity of solids is way higher than fluids, and therefore the time required to heat a solid is several orders of magnitude higher than a fluid. If we run the simulation at the fluid time-scale, which is necessary to perceive the changes in the fluid, this would lead to a insignificant increase of temperature in the solid. Supercycling treats the heat transfer in the solid on a different time scale. It storages the information of this problem and updates the solid temperature in each time-step of this new scale, treating the problem as different steady state cases in the fluid time scale. 

For this initial case, the simulation time is 0.5 s, with a variable time step starting at 1e-7 seconds. The supercyling interval is set to 0.05 s. The desired Reynolds number for the inlet flow is 10,000, and therefore the inner velocity, based on the pipe diameter and the fluid viscosity, is around 10.4 m/s.

Grid dependence test

Once decided all the other physical parameters, the first step in any simulation should be to select the appropiate basic grid size. In this case, we will track the outlet temperature and see what value of the grid size is enough to find convergence. 

These images show the mean outlet fluid temperature and solid temperature for three different values of the base grid size. Although they do not converge to the same specific value, they all are around a decent margin. It is clear that the solid temperature is going to be around 570 K and the fluid temperature around 335 K. Further refinement of the mesh should be done, but the current computer available already took one hour for the last simulation. Probably, a mesh grid size of 1 mm would be enough to pass the grid dependence test.

To optimize simulation time, the 3 mm mesh is selected for the rest of the project, as the academic purpose of the same only looks for quality accuracy (not quantitive) in the results.

Results (Grid size 3 mm):

When plotting the velocity profile at a constant z-plane around the exit, the velocity profile did not match the analytical solution. The reason for this is obviously choosing a coarse mesh. Although a further grid and time-step refinement is required, there are some conclusions to draw from the previous images. First of all, note how there is not change in temperature within the solid, due to the steady state problem solved by the sypercycling, and therefore this problem would not be modeling the real physics. Also, note how two layers (momentum boundary layer and thermal boundary layer) are growing through the pipe, due not only to the turbulence motion, but also the continuous heat influx to the wall. Finally, it seems like the fluid is fully developed at the exit of the pipe, as for the last quarter of the pipe there is no change in the fluid properties along the x-axis.


In a flow bounded by a wall, different scales and physical processes are dominant in the inner portion near the wall, and the outer portion approaching the free stream. The behaviour of the flow near the wall is a complicated phenomenon and the concept of y+ was formulated to distinguish the different regions. It is a dimensionless quantity, and it is the distance from the wall, measured in terms of viscous lengths.

In turbulent flow, we can divide the boundary layer into three sub-domains:

  • The inner layer, or sublayer, where viscous shear dominates
  • The outer layer, or defect layer, where large scale turbulent eddy shear dominates
  • The overlap layer, or log layer, where velocity profiles exhibit a logarithmic variation

Each one of these sub-regions has an specific required value of the y+ value, if all the physics want to be caught by the simulation. Based on these phenomena, the different turbulent models were created to simulate specifically one, several or all the three scales of the problem. In this case, the k-eps turbulence model was selected, and this model was designed primarily for turbulent core flows. K-eps turbulence model employs something called as wall function to simulate the flow in the near-wall region. Wall functions use empirical laws to circumvent the inability of the k-eps model to predict a logarithmic velocity profile near a wall.

In most high-Reynolds-number flows, the wall function approach substantially saves computational resources, because the viscosity-affected near-wall region, in which the solution variables change most rapidly, does not need to be resolved. However, it is inadequate in situations in flow at low Reynolds numbers, and the hypothesis underlying the wall functions cease to be valid.

In these three cases, the y+ value changes from 40 when the mesh grid size is 4 mm, to around 20 when the mesh grid size is 2 mm. Within this range, it is impossible to analyze the physics at the linear sub-layer, although it is obvious that it would be getting closer if we further reduce the mesh grid size. However, it is the right size to capture the logarithmic boundary layer using the wall-function and therefore is the right size for the k-eps model. Note that if we further reduce the mesh grid size, it is possible that the y+ value reduces below the threshold where the wall function is valid, and therefore the k-eps model would no longer be valid. 

Effect of Supercycle stage interval

In the previous calculations, the supercycle stage interval was set to 0.05 s, this is, the heat transfer problem in the solid was trated as a steady state heat transfer problem every 0.05 s. In this part, the simulation will be run changing this interval to 0.03, 0.02 and 0.01 s.

In the previous pictures we can see how the supercycle stage interval does not affect to the final value of the fluid or solid temperatures. There is, as expected, a change in the "transient", as the solid heat transfer is computed as different steady states. However, note that the intermediate values at this simulation are not valid to determine the real transient state of the problem. In this case, where only the final steady solution is important, all of the different supercycles stages would be valid as they all reach the same solution. However, what impact does changing the supercycle interval have in the simulation?

The computational time, for the different values is shown here:

SSI = 0.05 s

Summary of total time for:
           load balance                    =      0.07 seconds ( 0.02%)
           solving transport equations     =    328.25 seconds (81.08%)
           move surface and update grid    =      7.12 seconds ( 1.76%)
           update boundary conditions      =     21.54 seconds ( 5.32%)
           combustion                      =      0.00 seconds ( 0.00%)
           spray                           =      0.00 seconds ( 0.00%)
           writing output files            =     39.68 seconds ( 9.80%)

SSI = 0.03 s

Summary of total time for:
           load balance                    =      0.07 seconds ( 0.02%)
           solving transport equations     =    275.45 seconds (80.43%)
           move surface and update grid    =      6.21 seconds ( 1.81%)
           update boundary conditions      =     18.77 seconds ( 5.48%)
           combustion                      =      0.00 seconds ( 0.00%)
           spray                           =      0.00 seconds ( 0.00%)
           writing output files            =     34.60 seconds (10.10%)

SSI = 0.02 s

Summary of total time for:
           load balance                    =      0.08 seconds ( 0.02%)
           solving transport equations     =    287.56 seconds (81.04%)
           move surface and update grid    =      6.33 seconds ( 1.78%)
           update boundary conditions      =     18.72 seconds ( 5.28%)
           combustion                      =      0.00 seconds ( 0.00%)
           spray                           =      0.00 seconds ( 0.00%)
           writing output files            =     34.69 seconds ( 9.78%)

SSI = 0.01 s

Summary of total time for:
           load balance                    =      0.08 seconds ( 0.02%)
           solving transport equations     =    325.73 seconds (80.90%)
           move surface and update grid    =      7.00 seconds ( 1.74%)
           update boundary conditions      =     21.85 seconds ( 5.43%)
           combustion                      =      0.00 seconds ( 0.00%)
           spray                           =      0.00 seconds ( 0.00%)
           writing output files            =     39.64 seconds ( 9.85%)

Although the time difference here might not be huge, it is important to notice that we are simulating a coarse mesh, knowingly that an accurate simulation would take hours. Therefore, a 10-20% difference is quite relevant when trying to solve a thinner mesh. Notice that the higher supercycle stage interval does not lead to the smallest computational time, as it could be expected. The reason for this might be the huge information to be retained between each stage, and the important step the values has to take between one step and the next. Once the value is refined enough, then the computational time is indeed dependent on the stage interval. Therefore, there is an optimum value to make the simulation faster, without losing accuracy in the final solution.


- Conjugate Heat Transfer can be easily simulated using Converge Studio, if a fine mesh and the optimum supercycle stage interval are selected. 

- The supercycle stage interval method relates on treating the solid heat transfer as several stages of a steady state problem. Therefore, it is not valid if the transient behaviour of the system is needed (unless we select a interval small enough).

- The mesh selected in this problem provides a y+ value in the adecuate range for the turbulence model selected (k-eps with wall function).

- However, a thinner mesh is required to solve the problem accurately, as the current mesh does not pass the grid dependence test. A mesh around 1 mm should be enough to overcome this obstacle. Note however that the mesh can not be reduced progresively without consideration of the turbulence model. The wall function theory is not valid too close to the wall, and this must be taken into consideration, even if a more powerful computer is available.

- Finally, it was found that there is an optimum supercycle stage interval for minimun simulation time. This should be taken into account to reach an equlibrium between accracy and time in further simulations.



Projects by Jorge Martinez

The purpose of this project is to show the effect of initial temperature and pressure in the ignition delay in a combustion process. For this purpose, a Constant Volume Reactor and the corresponding network objects are created in Cantera, and the combustion process is s Read more

The purpose of this project, is to setup and analyze a transient shock tube simulation using Converge Studio. The project will analyze how the interaction of the original shock waves and the reflected waves affect the fluid in the tube, and how the computational mesh ha Read more

This project objective is to simulate the Prandtl Meyer shock wave phenomena using Converge Studio. First, a quick literature review about shock waves and their boundary conditions is provided. Then , the problem is set up and solved, focusing in how the different param Read more

The purpose of this assignment is to create a Python program including a Multivariate Newton Rhapson Solver, to solve a non-linear coupled differential system. This method is really useful for stiff systems, where the explicit solver are unstable. The system of equatio Read more

The objective of this part of the project, is to simulate the transient flow through an elbow pipe with a throttle valve in the middle. This valve will be rotating from zero to 25 degrees, and then stay steady.  Case Setup. In the steady state part of the project Read more

This project purpose is to simulate the flow over an elbow body that contains a throttle using CONVERGE Studio. In this first part of the project, an steady state analysis will be set up. This means that the throttle will not move. This case helps set up the real analys Read more

In this challenge, the efficiency of using a heat recuperator to pre-heat the air is analyzed. For that, we simulate a furnace burning methane and air mixture, and we analyze first how the pre-heating affects at the AFL, and then the total heat/work that could be extrac Read more

This project main objective is to calculate the Adiabatic Flame Temperature using Python and Cantera. In the first part of the project, the effect of the equivalence ratio for the methane combustion in a constant volume chamber is analyzed, and the python and cantera re Read more

This projects aims to simulate a backward facing step flow using CONVERGE Studio. The flow is creating when a not reacting specie, air (23% O2 and 77% N2 in mass fraction), suffers a pressure gradient between the ends of the channel. The velocity, pressure and recirulat Read more


The End