I’ve created a project to simulate the wind load effects on solar panels on the roof of a building. As we can see in the pictures below, each solar panel is secured by two plastic frame (in blue color, shell shaped).
I used to simulate the project by using Incompressible (steady state) setup, however, an engineering from the following website stated that we must test the design in gusty, turbulent airflow. So, I tried another simulation using Incompressible Transient Mode to simulate the wind load effects created by turbulence. https://www.cppwind.com/wind-effects-on-solar/
Therefore, the objective of this project is to see the wind loads (especially upward force created by gusty, turbulence wind in the rear frame) acting on the design setup, so that I can determine the minimum number of sand bags I need to put inside the plastic frame in order to prevent the structure from blowing away by strong wind.
The result indicated that the upward force (Z-force) acting on the back solar panel frame setup is about 2400N.
However, I’ve got some questions:
1. I’m not a professional wind engineer, could some expert tell me if my settings are OK? 2. The force plot looks quite steady (a straight line), but actually, the wind should be gusty and turbulence. How could I modify the setting to get the correct answer? 3. Is my mesh too fine or just Ok?
For simulations that reach Mach numbers > 0.3, the compressible analysis type is suitable.
Make sure to include the viscous forces too.
What about simulating half the model to save resources? It seems symmetric to the plane normal to the x-axis. Then you could refine your mesh even more. (For example, this project uses Symmetry combined with the Hex-dominant parametric algorithm: Hex-Dominant Parametric Meshing of Front Wing | SimScale)
With your current Simulation Control settings, the run is set to perform 15000 loops. What about trying 1500 instead? If this doesn’t converge by then, you can increase this end time and continue the run afterwards (have a look here: Can I Continue an Existing Simulation Run in SimScale?)
I went through the mesh refinements and didn’t find an Inflate boundary layer for the body (correct me if I am wrong). This is important for the simulation, so maybe you should considering adding this. (What is y+ (yplus)?)
Hi @gkwok. I would like to provide more comments about your Incompressible (mid) simulation.
You have good mesh (very small, ~820 kCells), hence you simulation should be done in couple of minutes only. But you used ~63 core-hours.
Please, in Simulation control, set Potential flow initialization to yes.
In Simulation control, you have End time cell, which is not i seconds, but in steps. For starting, put it to 500.
In same dialog, put delta t to 1. That way you will have 500 steps initial simulation. If you wish, you can extend that to more steps after reviewing the results.
In Result controls, you have to define ‘Rotation point’ for your Front / Rear blocks. Otherwise you will have wrong momentums (torques) on those blocks. In current setting, your blocks with panels will be ‘moved’ around that 0,0,0 origin.
That kind of structure will be subject of strong vortex shedding, so you may expect, even for Incompressible steady state simulation residuals and Forces fluctuations.
Currently mesh is so small, that you need not to use symmetry (in my opinion).
