Convergence issue

Hi there,

I have an issue with a simulation I am trying to run, the Uz, Uy an pressure don’t seem to be converging.

I have tried to adjust the relaxation factors to manual with the default settings, and i have also tried reducing the residual controls for velocity and pressure from 1e-6 to 1e-8 and nothing has improved.

I understand that it is possible to increase the run time to improve convergence however the run took 180mins to reach 460 secs simulation time.

To also add i have tried to adjust the mesh but it did not help, only made the simulation time take longer, producing less simulation time results.

If possible i would like help on how to improve the convergence of results and if possible reduce the rate of convergence, I might add that i wish to use the standard mesher as i want to run the model with more complex geometries such as a helical model, so a structured mesh may not bee the best ( I might be wrong about this?)

Link to the model is here: SimScale Login

Thank you

Hello ss02150

I have a few ideas regarding your simulation.

I personally think that you will need more run time. Usually, you would run simulations for at least 1000 Iterations.

To achieve this you maybe make the wind tunnel a bit tighter to save cell numbers.
You can also, try to add an initial velocity under initial conditions. with that the simulation will be initialized with a velocity that is closer to the velocity at the end.

Also to check for convergence at your building you may want to check a result control item such as a surface average at the back of the building. With that, you can check the convergence of the forces/pressure at the building.

Best regards
Sebastian

Hi @SBlock,

Thank you for your help, with regards to your recommendations, the domain size I have has been based off literature i have looked into as part of my project so if possible i would want to try and keep the domain the same size.

In terms of the initial conditions would you recommend i set this as the ABL wind profile defined in my velocity input?
With a previous run i had completed the forces converged and became steady, however the residual plot did not meet the recommended value of 1e-3, can i still use the force result even if full convergence was not met?

again thank you for your help and your fast response, I appreciate your time.

Hi ss02150

maybe you can have a quick check of the domain size and see what the difference in result is, if there is no difference I would say you can stick to the smaller fluid domain.

For the initial condition, you can just set a mean value, so I would go with a good average value of your ABL (free stream velocity) .

In regards to the residuals, it depends on the results you are interested in. If the residuals for example high further away from the building, it won’t have an influence on your result. Therefore I would focus on the results you are interested in.

Best regards
Sebastian

Hi @SBlock,

I will give this a try and update you once i have results, one last question, how do i check the residuals in the near building regions, thank you.

Hi ss02150,

unfortunately, there is no direct way to display the residuals.

Therefore I would take the surface average result and compare that to the average residuals convergence. I guess that this is a good workaround.

Best regards
Sebastian

@SBlock
For this residual plot

the results for the surface data for pressure

and the following for force plot with the point at the base

It seems that the results are converged even with the residuals not converging, can they then be used or do i need to get the residuals lower?

I am not completely sure what you are trying to simulate but if I am not wrong it is a block at an angle of 45° degrees (angle of attack) right?

If it is so, most likely the reason your solution does not “converge” more is that it cannot converge more. You are performing a steady-state analysis of a box at 45 degrees of AOA. There is flow separation. The solution does not have a steady-state solution but a number of “solutions” that come close by, because the phenomenon is inherently transient. Therefore, your results are called “quasi-steady state”. The oscillations you see in the residual plot is the solver trying to come by with a solution that does not exist. Image a simulation of an airfoil at 18° AOA. There is flow separation. The airfoil is at stall. There’s buffeting. This is a transient phenomenon. Using a steady-state solver on this problem will cause the solver not to find a satisfying converged solution.

Solution: Simulate using a transient state approach.
Do not try to (not recommended): Use the quasi-steady state solution (the one you already have) as the definitive result. If you are measuring lift and drag, you will obtain different results with the transient approach.

@SBlock, my suggestion is for SimScale to write a tutorial / technical text about this behaviour. This should be like the 10th time I see this issue addressed in the forums :slight_smile:

Best regards,

J.A. Gutiérrez.

1 Like

@ss02150 as I see the residuals right now, after more iterations, I would as @jairogut suggest running a transient analysis.

@jairogut yes that might be a good knowledge-based paper, thanks for pointing this out. Something like
“How to detect transient effects in steady-state simulations.”

1 Like

Yeah, I would call it something like this: When to switch from steady-state to transient -- CFD Online Discussion Forums. Although that forum post does not contain all the information we have been discussing.

1 Like