The Engineering Problem:
An exposed building facade is being heated up on one side by sun. Within it we have an air socket that cools the facade with convection motion. The whole wall looks like a “sandwich” with an air gap. The air gap is open on the bottom and top allowing air to freely move.
From left to right in the figure 1:
- 3 mm steel sheet
- Air gap with 150mm thickness.
- Steel structural mesh attached to the steel sheet through 8mm x 8mm square arms.
- 200 mm Styrofoam layer
- 20 mm ABS plastic layer
The model designed to represent the building facade is a reduced model of what would be a real wall. That was made to save computational time and cost. The dimensions are 0.4 m x 0.4 m x (air gap + 0.231) m, where the air gap has 150 mm. An extended volume for the air - as can be seen in the green region in figure 1 - was used in order to have a better continuity of the fluid flow through the domain.
A hex-dominant parametric operation was used to mesh the geometries. Refinements such as Surface, Region and feature refinements were made to assure the good quality of the mesh.
The final mesh has a total of 6’844’659 elements.
Msh detail in the image below:
A laminar steady-state conjugate heat transfer analysis was performed to study this model. The model contains 4 different materials, which are: air, steel, styrofoam and abs plastic. The ambient temperature was assumed to be 25 degree celsius.
The boundary conditions are shown in the next figure:
As shown above, it was setted the outside surface of the metal sheet with 50°C, what is considered a high temperature which would occur in extreme conditions, e.g. in a hot summer day.
The bottom surface in the air domain - which is the one in green in the figure above - is a velocity inlet boundary condition with a component in the y axis direction. Three different values was tested, 0.05m/s, 0.1m/s and 0.2m/s. The top surface in the air domain was set as pressure outlet. The surface in the abs cover which would be the internal surface of this facade was set as wall with external heat flux specified by a heat transfer coefficient and an ambient temperature of 25°C. Other faces were assumed to be either symmetry (in x direction) or adiabatics.
From the images above it is possible to see that the air as it passes close to the heated steel sheet it gets faster and goes up as it was expected. However, we see that especially for the 0.05 and 0.1 m/s simulations, there are regions of very slow velocity.
From the next images it is possible to see that it is happening some recirculation inside the air domain. That doesn’t happen for the 0.2 m/s air velocity. So it is possible to say that there is a velocity in the z direction which is enough to don’t get this back flow in the domain. Back flow which appears to maintain the balance of the system.
As said before, from the images above we see that recirculation is almost zero for the 0.2m/s air velocity.
We also have results for the temperature distribution as shown in the images below:
The images above shown a slice in the middle section of the model in y direction. It is possible to see the temperature distribution from the heated metal sheet, how it decreases through the square arms and also that there is a slightly difference in the temperature contour in the styrofoam and abs regions. This can be seen also in the next graph, which shows the temperature distribution in a line in y direction starting from the heated metal sheet coming through the square arms into the styrofoam and abs blocks.
From the graph we can say that the velocity of the air which flows through the air gap has influence on how the temperature decreases in the solid bodies. The inflection in the three curves shows the transition between metal and styrofoam material. The temperature stabilizes faster as air velocity increases.
This demo proved to be a very complex system to simulate as the results inside the air domain are dependent on the flow velocity and probably on the air domain size. Some back flow can happen where we have placed the outlet surface. Some reverse flow can be tolerated, but will have an effect on mass conservation and thus on the final results. So it is highly recommended that it be minimized or eliminated.
A study can be done moving the outlet position further upstream and comparing the results with the ones in this simulation, in order to see if those backflows are minimized also for the slower velocities.