I'm trying to simulate the 2D flow around a RAE 2822 transonic airfoil.
The first simulation was fine but schock wave was very weak so I decided to refine the mesh. With the second mesh, simulation gave me a strange behaviour with a "ball" of negative pressure at trailing edge.
The two simulation are cloned and the only thing I changed was the value of the mesh size around the airfoil.
Do you have any suggestion to solve this?
Solved! Go to Solution.
Could you share a little about the setup, what BC's you have assigned for instance? What turbuence model are you using also?
Also, could you share an image of the mesh as it is now?
As this is compressible I would try with a mass flow rate, and total temperature at the inlet. You should not assign both a flow rate and a temp on the same surface.
Use the scenario environment pressure to adjust the pressure if needs be. The outlet should be fine as unknown.
The mesh looks OK.
It might be worth considering the SST turbulence model but for now just try those changes and also switch to ADV5 (Solve -> Solution Controls -> Advection) and see how it runs.
Thank you, I will try.
ADV scheme was already ADV5.
For mass flow rate in a 2D simulation, I will asume that the depth in the third direction of the mesh is 1 m?
CFD assumes a unit thickness so it depends on the units you have assigned. If you are in mm, yes it will be 1mm thick. I hope that helps.
With mass flow rate, pressure and total temperature the simulations seems going good, shock wave is still weak but I think it mesh related.
I also switched to SST.
refining the mesh more deeply causes instability of the solver (ADV5, SST) also with mass flow rate/total temperature BC.
I solve this problem running an incompressible simulation for the first 1000 iteration and after swtiching to compressible. After 5000 iteration it's stable and going slowly to convergence.