[MNMK]

Originally Posted by Gert-Jan

- You have a FINMES error. This means Final Message. Not very helpful
- You use k epsilon. Better use SST
- Why do you use a physical timestepping. Better use auto timescale and let CFX determine the size based on occurring phenomena.
- Your case is not converging at all. Did you create a backup just before the crash? If not, please do. This might help in finding the cause.
- The modelling approach you use, with translational peridicity works pretty will, if the tubes are straight. Then the velocity in and out have a change to make sense, provided there is no huge recirculation and backflow in the outlet, because that will appear at the inlet as well, which the solver does not like. For the same reason, it is common practice in CFD in general to move outlets downstream such that objects of interest do not influence outlets and vice versa. In your geometry, you have a similar problem. I think there will be many recirculations just in front of your outlet that will affect the flow in the inlet. Therefore I am not convinced your approach will work for this geometry.
- Did you try to perform a simulation on a segment instead of full 360°? This might help.
- Did you try to make the interface on the smallest diameter instead of the largest diameter. I would expect that to work better since the recirculations close to the outlet will be reduced.

Hi,

I have tried SST Model but I received the same fatal error.

I have tried the Auto timescale. However, I was faced with the same error. Therefore, I chose the best Physical Timestep which the calculation had the best residual.


It would be great if you suggested a solution.

best,

[Gert-Jan]

What about my last suggestion? Please try this first.

[MNMK]

Originally Posted by Gert-Jan

What about my last suggestion? Please try this first.

Surely, I will try the suggestion. Do you mean I make an interface in in/outlet with a diameter like a straight duct.Infact you want to ignore the recirculation in the wave zone. To be sure: Don't you think it has a negative influence on result?

[Gert-Jan]

You have a tube that looks like a vacuum cleaner hose.
From that, you select a section such that inlet and outlet are on the large diameter.
I would take a section such that inlet and outlet are on the small diameter.

[MNMK]

Originally Posted by Gert-Jan

You have a tube that looks like a vacuum cleaner hose.
From that, you select a section such that inlet and outlet are on the large diameter.
I would take a section such that inlet and outlet are on the small diameter.

Hi,

I have tested your suggestions.
1.With a smaller diameter--> I have got the same fatal error. In fact it did not work.

2.I have reduced the geometry to 45° instead of 360° with periodic boundary conditions, as I could guess I did not work as well.

I am looking forward to other advice.

regards,

[Gert-Jan]

- make several backups just before it crashes, by clicking on the backup button in the top ribbon of the solver manager. Open them in Post. What do the results in these backups tell you? Is the velocity developing weird, or pressures, or something else? What makes them crash?
- I would take a segment of 5° instead of 45°, or even smaller.

[MNMK]

Originally Posted by Gert-Jan

- make several backups just before it crashes, by clicking on the backup button in the top ribbon of the solver manager. Open them in Post. What do the results in these backups tell you? Is the velocity developing weird, or pressures, or something else? What makes them crash?
- I would take a segment of 5° instead of 45°, or even smaller.

I will send you the back up.
I do not understand what can be better at 5° than at 45° ?

[Gert-Jan]

The recirculations will have a 3D character. When the segment is just 5°, there is less space to develop in 3D.
However, if these eddies are the phenomena that you want to study, then these are important and your whole approach is wrong. Then you need to step away from this approach. It would be better to add straight parts at inlet and outlet.
But that depends on the question that you want to answer when doing CFD. And I don't know your question yet.

[MNMK]

Originally Posted by Gert-Jan

The recirculations will have a 3D character. When the segment is just 5°, there is less space to develop in 3D.
However, if these eddies are the phenomena that you want to study, then these are important and your whole approach is wrong. Then you need to step away from this approach. It would be better to add straight parts at inlet and outlet.
But that depends on the question that you want to answer when doing CFD. And I don't know your question yet.

I have made some backups, and I have also imported them to Post. I should say, I have tried, by looking at the Residual trend during the calculation , to reduce the time scale from 6e-4 to 1e-4.Because I see the more fluctuations in my DP as a monitor point during my calculation. I have attached result photos. The pressure changed dramatically. As can be seen in the third photo, the direction of the velocity vector will be reversed.!! Is it come because of higher Time steps or there changes?? Is there any advice about how I can reach the right and convergent result for such a case?

[Gert-Jan]

The problems you face have nothing to do with time step size.
You want to study the flow in a corrugated pipe using translational periodic boundaries.
But your curved outerwalls are much to close to the periodic boundaries. The curved outerwalls create recicurlations close to the outlet, that as a result end up in the inlet since both are connected. Therefore you will never find a converged and reliable answer.
As I mentioned before, you should step away from this method unless you add straight parts at the inlet and outlet of at least 5D length. That will reduce the effect of the recirculations.

[MNMK]

Originally Posted by Gert-Jan

The problems you face have nothing to do with time step size.
You want to study the flow in a corrugated pipe using translational periodic boundaries.
But your curved outerwalls are much to close to the periodic boundaries. The curved outerwalls create recicurlations close to the outlet, that as a result end up in the inlet since both are connected. Therefore you will never find a converged and reliable answer.
As I mentioned before, you should step away from this method unless you add straight parts at the inlet and outlet of at least 5D length. That will reduce the effect of the recirculations.

Dear Gert,

I am not convinced of your idea. I have tried a better timestep (smaller) and it works. It takes longer to converge, about 5000 iterations. Please look at the attached photos. I appreciate it when you tell me your opinion.

regards,

[ghorrocks]

You have to be careful when using very small time steps as that can artificially reduce the reported residuals and make the simulation appear more converged than it actually is.

If you want to see if your small section is accurately modelling the flow then compare the results from your model to a model 10 times longer. Does it give 10 times the pressure drop?

But Gert-Jan is correct when he says that putting periodic boundaries in regions where separations exist is a bad idea and will lead to convergence problems. You should always try to avoid putting boundaries in separations as it always leads to problems.

[MNMK]

Originally Posted by ghorrocks

You have to be careful when using very small time steps as that can artificially reduce the reported residuals and make the simulation appear more converged than it actually is.

If you want to see if your small section is accurately modelling the flow then compare the results from your model to a model 10 times longer. Does it give 10 times the pressure drop?

But Gert-Jan is correct when he says that putting periodic boundaries in regions where separations exist is a bad idea and will lead to convergence problems. You should always try to avoid putting boundaries in separations as it always leads to problems.

I appreciate your feedback. I would like to mention some points for other people who have the same questions in the forum :


1.I tried this method with a flat cylinder and I compared the results with another software (Pressure Drop calculator) and the results were so close to each other.

2.Also, I have considered the monitor points (Velocity in/out, Pressure Difference) to monitor the convergence. They were, after 4000 iterations, constant.


However, I try to evaluate the result through experience or longer Geometry in simulation.

regards,