Learning Forum

[jon]

Hello folks,

I am simulationg a relatively simple problem where 5 slow jet streams (inlet speed under 1m/s) enter an open domain as shown in the following images. The short horizontal walls just at the inlet have a free slip condition.

 

 

I monitored the drag coefficient at the horizontal walls that enclose the 5 inlets to verify convergence. I use:

• k-omega SST
• SIMPLE Scheme
• Second order pressure
• 1st order Momentum, turbulent kinetic energy and specific dissipation rate
• Tubulent intensity at inlet is 5%, turb. viscosity ratio is 10 (standard value)

My question now is: In the graph below you can see the graph of the drag coefficient. After a while it starts fluctuating a lot with a relatively constant amplitude and frequency. Although the values might still converge, I fail to explain where these fluctuations come from. I assume that I might have caused them by prividing a "bad" problem and caused instabilities. What would be a feasabile approach to educe the effect. Btw, as shown in the second graph, the problem is getting worse when using higher oder momentum equations.

 

[NickFL]

 

It is difficult to say. You will have to do some studies to determine if it is a numerical problem or if it is a real physical phenomenon.

Case for physical phenomenon: you have five planar jets that are confined in a small compartment before injection into the environment. Have you looked for journal articles for similar cases? I could imagine that with these five jets potentially interacting with one another, that there would be some natural instability. This would show up in a steady-state model similar to what you are seeing here. If you transitioned to a transient model maybe you could see some of these vorticies that are formed and shed which leads to this oscillation. A 10% change would not be unrealistic.

Case for numerical problems: I really don’t like the mesh near the inlet. It jumps in size and then shrinks again. Can you subdivide this out and get better control over this area (maybe use virtual topology if you don’t have access to the geometry)? I would also expand the mesh not just downstream but allow for the jet to expand. See the image below (note the mesh itself is not adequate, but I wanted to be able to show how to divide it better). What is the appropriate spreading? Well I would use at least what a typical jet would have at the given Re. There are many papers with it, but one I go back to is: https://authors.library.caltech.edu/5172/1/KOTjfm76.pdf . Thirdly, you mention the inlet turbulence values. I would not use turbulence and intensity. Instead switch to the hydraulic diameter form. Here you can specify the value height of each nozzle as the D_h and it will likely give you a better estimate of the incoming turbulence quantities. This may also remove some of the oscillation intensity.

 

 

[jon]

Thanks fo the great input, I appreciate it and it helps a lot! I'll come back as soon as I have some further results!