How to get system convergence

  • 54 Views
  • Last Post 6 days ago
  • Topic Is Solved
trippleD posted this 2 weeks ago

Hello everybody,

I'm doing a simulation of the flow in an annular gap. The inner cylinder is modelled as a rotating wall and the outer one is a stationary wall. The left and right side are stationary walls as well. All in all, it is a closed system. I'm using the realizable k-epsilon model with enhanced wall treatment. 

For the convergence, the resiudals should fall by a magnitude of 10^-3 respectively 10^-6. I do a steady state simulation with 2000 iterations. But i don't reach the values to say, that my system is converged (please see the attached picture).

 

What can i do for reaching a converging system?

The zipped project was to big to upload it here, you can download it from the link below:

CFD_Simulation_model

Please tell me, if you need additonal information.

 

Thanks for your help,

Order By: Standard | Newest | Votes
abenhadj posted this 2 weeks ago

Please use coupled solver with pseudo-transient. We do not look into attachments as ANSYS Staff.

Best regards,

Amine

trippleD posted this 2 weeks ago

Thanks for your answer. I will try it. The options for Pseudo Transient Options stay Default?

 

Okay, i didn"t know that. But here it is explained how to add a project. For what reason?

abenhadj posted this 2 weeks ago

that applies for non ANSYS Staff: other community members. If you want ANSYS Staff to help you need to add description and screenshots.

Best regards,

Amine

trippleD posted this 2 weeks ago

Ok. I have an additional question. Why do you reommend the coupled solver with the Pseudo Transient?

abenhadj posted this 2 weeks ago

That is written in the documentation: Momentum equation + pressure-velocity corrections are done in coupled fashion. It converges quicker and uses an additional implicit under relaxation factor for all cells by using low order time marching approach to solve steady state problem.

Best regards,

Amine

trippleD posted this 2 weeks ago

I've just perfomed round about 400 iterations.

I there a way to accelerate the convergence behaviour.When looking at the picture it will take forever to reach convergence.

abenhadj posted this 2 weeks ago

Run for more iterations and we will see. You can start by using fixed time scale corresponding to 0.1/angular velocity or 0.01/angular velocity

Best regards,

Amine

trippleD posted this 2 weeks ago

I have done a few more iterations as you can see in picture below:

 

So can i say that the system is converged. The simulation was running with a timescale factor of 1. Or should i try a new simulation with the recommendation from you? What did you mean exactly. Time Scale factor = 0.1 or = (0.1/agular velocity)

Thanks for your help

abenhadj posted this 2 weeks ago

To judge convergence you better monitor some key variables or integral quantities as well as check the imbalances under flux report. If all are good then you can say that it is converged.

Best regards,

Amine

trippleD posted this 2 weeks ago

Okay, i check some variables and they look like they make sense. 

It is a close system, so i think the zeros are good an the value for interior fluid is the mass flow due to rotation. The inner cylinder is rotating with 52,36 rad per second. the inner radius is 0,025m. The maximal velocity is then 1,309m/s. So the maximum velocity i get from the reports is:

Is it normal? 

So do you think the system is converged? I want to hear your opinion.

Thanks again, you are helping me a lot.

abenhadj posted this 2 weeks ago

You need to monitor the values while the solution evolves: Say like volume average of (tangential) velocity or velocity at certain point (or temperature or wall shear stress or torque or anything relevant for your applicaiton).

You need to build up your opinion. I am helping you to do that. 

Best regards,

Amine

trippleD posted this 2 weeks ago

Okay, so i have to do the simulation again and monitoring the values you have mentioned?

 

abenhadj posted this 2 weeks ago

Yes.

Best regards,

Amine

abenhadj posted this 2 weeks ago

 Or continue running after creating the required reports.

Best regards,

Amine

trippleD posted this 2 weeks ago

Okay, i have done the report for the tangential velocity and start the simulation. I will let you know when it is finished. 

During the meantim. Let"s say the system is converged and i start my simulation with the data of the converged system. How many iteration do i need than for getting good results? Or is the simulation finished when the system is converged?

abenhadj posted this 2 weeks ago

You define when the run finishes. The software just finishes run to the condition you set: Residual tolerance, monitor convergence or whenever you hit stop. So that is you who needs to care about all that.

I recommend doing some standard tutorials.

Best regards,

Amine

trippleD posted this 2 weeks ago

I think i was misunderstood. but now it is clear. I have done some tutorials, but the cfd is such a big topic

trippleD posted this 2 weeks ago

I continue the simulation. It is still running, but i want to give you an intermediate status.

As you can see, the volume average of tangential velocity isn't changing. So i think, the system is converged, right?

abenhadj posted this 2 weeks ago

You need to make your judgment on your own. IMHO the profile looks okay. Check if you have any mass imbalances in your domain. Report mass of the whole volume and examine its evolution during iteration.

Best regards,

Amine

trippleD posted this 2 weeks ago

I do the judgement on my own, but i want to double check it with someone who has experience with it. Okay. so all in all i can say, if the values aren't fluctuating anymore, the system is converged.

Is there a possibility to export the values of the residuals ?

abenhadj posted this 2 weeks ago

You want to export them into file or you want to visualize them as contour variable?

Best regards,

Amine

trippleD posted this 2 weeks ago

It would be the best to export them into file to read them in Matlab

Thanks for your hep

abenhadj posted this 2 weeks ago

You require an UDF for that. Alternative is to store the non scaled residuals and export to ASCII. Scaled residuals as workaround can be exported if you write transcript of Fluent run. You need later to remove all unnecessary lines.

Best regards,

Amine

trippleD posted this 2 weeks ago

Can you explain it more in detail how it works (export the scaled resiudals)? Thanks a lot.

abenhadj posted this 1 weeks ago

In Menu File>Read>Start-Transcript, run the case then Stop that Transcript again.

Best regards,

Amine

  • Liked by
  • trippleD
trippleD posted this 1 weeks ago

Thanks a lot Amine, that works very well

Because the simulations are very time consuming, is there way to extract the from resiudals from saved simulation which are already done?

abenhadj posted this 1 weeks ago

As i write earlier you require an UDF for that. Alternative is to store the non scaled residuals and export to ASCII: I would go for that. Scaled residuals as workaround can be exported if you write transcript of Fluent run. You need later to remove all unnecessary.

Best regards,

Amine

trippleD posted this 1 weeks ago

Can you show me both? The UDF and the export of the non scaled residuals.

abenhadj posted this 1 weeks ago

UDF: Sorry I cannot show.

To export non scaled residual you first enable them to be stored:

In the the Fluent console you type /solve/set/expert and then when it is asked for Save residuals for post-processing you confirm with yes. You ran one single iteration and you will the non-sacled residuals available. Afterwards you go (GUI) File>Export you select type ASCII and then the residual variables.

Best regards,

Amine

  • Liked by
  • trippleD
abenhadj posted this 1 weeks ago

You can alternatively go unde menu plot (TUI)>residuals-set then plot-to-file. Afterwards you ran whatever iterations you want

then you under menu plot type res and then answer with yes for all equations.

Best regards,

Amine

  • Liked by
  • trippleD
Show More Posts
Close