Not attaining convergence-External flow
 

Hi
I am doing a study on the external flow of a body in two different conditions:
1. closed body (eg: car with closed windows)
2. Open body :The body has a few openings which allow air to flow internally and pass through it. (Eg: just like car with open window)
I am trying to calculate the Cd value in both conditions. For this, i am using K-omega sst solver(as observed in literature) with the segregated flow in steady state. I tried the solution with tetrahedral mesh and didn't get convergence. Then I moved onto the polyhedral mesh. I tried different mesh refinement methods to effectively capture my geometry. The geometry is a bit big, so the number of cells are quite high (16million). There is a lot of fluctuation observed in residuals. I am not getting convergence. As mentioned by few people, if I have to take the Cd value when the fluctuation is quite low , both conditions are in the same range which can not practically be possible. So please suggest me some ways to obtain convergence. The velocity used for this problem is 100kmph.

Thank you in advance. :)

Did you try trim mesh, if it is a flow dominated unidirectional flow.....

Sent from my Redmi 3S using CFD Online Forum mobile app

I guess the problem is not the mesh and is the type of formulation (steady state) and the boundary conditions

Hi Krishna,
Can you please post picture of mesh model.
As mentioned external flow case, I hope trimmed mesh will be probably best option. Have less numerical error with better convection calculation.
To lower numerical diffusion, better capture the wake region with refined volumetric control box.
I think you can go up to 25-30 million cell count, may reflect better prediction.
Scalar monitor may help to observe convergence, don't depends on residuals only.
How much % variations you observed in residuals?

Sent from my Redmi 3S using CFD Online Forum mobile app

Thank you for suggestions. For further refinement in mesh I need a system with better processor. Right now I am at full usage of available resources. The variations in residuals are high.. one is in 10^-4, the other in 10^-2

Sent from my KIW-L22 using CFD Online Forum mobile app

you should also be looking at history plots of other reports like lift and drag and maybe other reports.
most flow is transient even with steady boundary conditions and there are eddies and fluctuations that keep the residuals high in many cases.
a finer mesh might even make the residuals higher since it finds more fluctuations.
it is quite common to run external aero cases in steady first then carry on in unsteady to ensure the fluctuations are more accurately captured and then average the drag etc and many users are now using des to better capture the flow which must be run in unsteady mode.
so your results might be fine as they are but until you run unsteady you wont know.
you can also look at where the fluctuations are occuring with a scene of each residual field by turning on temporary storage etc