Hi, at what level the residuals oscillate in your case? Could you attach a print-screen reporting changes of their history?

Dear Zahra Kowsar ,

In all numerical simulations you should consider the following steps to achieve the best convergence:

- Notice in the flow regime, Laminar or Turbulent. Considering that, select the Proper governing equations.

- Mesh is very important factor. The structured mesh give rapid and better convergence. If it is not possible to use structured mesh, use the meshes with the least skewnessour highest possible quality.

- Separate your domain into different regions. the more sensitive regiones should be meshed by finer elements. the rest, is better to be meshed by larger ones.

- Work on time steps. it is very important.

- Generally, Ansys assign zero value as initial values. Changing the initial value is helpfu, sometimes.

- Notie on your boundary conditions!

to kamil kaminski

their maximum change level is 30% ,this occurs only for u and w

to farhad sadegh moghanlou

thank you for your comprehensive description,is was very good, i think my problem is meshing, i studied below sentence in cfd-online site:

"Oscillations during a steady simulation can also occur if your geometry has some symmetry but your grid is not symmetric "

i have two question:

i dont know how i can create a symmetric grid,while my geometry is complicate.

is the symmetric grid the same structured grid?

thanks

The change of one third is definitely not enough, I would expect a change of at least three orders of magnitude for a convergent solution. If advice from Farhad Sadegh Moghanlou does not solve your problem, you may also consider obtaining an initial solution using the first order schemes and next, if solution is converged, switch to second order approaches. In my work I use Fluent so I am not sure if CFX offers such option.

thanks a lot Mr. Kaminski, i'll do it

Zahra Kowsar : You told, that your domain is rather complex in geometry. And I assume, that you try to run your calculation in steady-state mode (CFX pseudo-transient method).

Than the question is, whether at all for this complex shaped domain a steady-state flow condition really exists for this type of application? This is not guaranteed. Transient flow features might be so irregular and pronounced, that the CFD solver is not able to converge to a statistical steady-state result for the used integration time step.

In this case the usually observable CFD solver behavior is like this:

1) small (delta t) integration time-scale:

The solver iterations are run robustly. Convergence progresses reliably - up to a certain point. If a steady-state solution exists for the type of flow, you can arbitrarily deep converge. If not, residuals for a number of equations stagnate and start to oscillate. This can than be a sign of the onset of resolved transient flow scales, which than lead in the flow domain to a differently predicted flow field from one iteration to the next.

2) one tries to increase the (delta t) moderately to higher levels:

With the increased dt we are now integrating ("smoothing") over the very small transient flow scales, since those can now no longer be resolved, since they are smaller than the applied integration time scale. But the increase of dt is for the risk, that the numerical accuracy of the time integration is reduced ( order of dt°2 for a second order time integration method). In the pseudo-tansient time scheme this is usually not an issue, and quite large time scales can be used with success, thereby integrating over larger and larger transient time scales, which might exist in the flow of interest and trying to predict a potentially existing steady-state flow behavior in the statistical sense. So you could try to increase the pseudo-time-scale in your simulation and see, whether that helps to suppress the small-scale transient features in your flow of interest.

3) further increased dt to rather large values:

By further increasing the time-scale to rather large values (in the order of seconds), you might experience from some point onwards numerical instability of the CFX solver. The numerical disturbances from using such large time-scales are becoming that large, that they cannot be effectively be reduced by the iterative solution algorithm anymore. The result is usually solver divergence.

So if there is no range like (2) where the increase of the integration time-scale leads to a statistically steady-state solution and reliable convergence, than most likely the underlying flow is too chaotically transient in flow nature. In that case the remedy is:

1) carry out a full transient flow solution over a representative period in time for flow development

2) once the flow is fully developed --> activate time-averaging of results in the CFX flow solver

3) run the flow averaging in full transient mode over a representative period in time and a statistically relevant number of timesteps (several thousands).

4) Now analyze the time-averaged CFD result.

Hopefully this explanation is helpful to you.

Best regards,

Dr. Th. Frank.

to Dr. Th. Frank

yes, your reply was very complete and that was my fault,thank you very much Dr. Th. Frank