Simulation Error


#1

Hi,

I am currently working on a CFD project with the CAD of a vehicle that includes external and internal flows.
I had previously run 2 simulations and they both worked. I have uploaded 3 new CAD´s with geometry changes, the meshes were created accordingly, but when I want to run the simulation with the same parameters, none of the 3 meshes run. I have tried re-modifying and re-uploading the CAD but the same problem is obtained.
The project link is: https: //www.simscale.com/projects/cmartiso/uni_-_rp/
Could someone please help me out?

Thank you!
Carla


#2

Hi @cmartiso,

currently running a simulation and getting back to you as soon as the run has finished.

Best,

Jousef


#3

Hi @jousefm

That´s great! Thank you :slight_smile:

Carla


#4

Hey @cmartiso!

You should have an email - shared two finished runs with you.

P.S.: Make sure that the turb. kinetic energy and the dissipation rate are calculated properly. For more information, please have a look at: Defining Turbulent Boundary Conditions

Best,

Jousef


#5

Hi @jousefm!

Thank you for your help! I have read your turbulent constants, and with the equations and some wind tunnel data I have obtained different constants, will try them out!

Thank you very much! :slight_smile:
Carla


#7

Hi @jousefm

I need your help again regarding the same problem, I keep on having simulation errors. If you look at the same link I gave you initially I have run 4 more simulations with different k and w constants but the residuals looks too similar, making me think that there is another problem. Do you have any suggestions?

Thank you for your time!
Carla


#8

Hi Carla,

that’s not an error but a message stating that you just need to increase the runtime. In any case I think that a run with 10,000 seconds is too much and you can see if 3,000 are enough and make sure that the forces or residuals do not change significantly after a certain amount of time.

So to answer your questions: Increase the Maximum runtime [s] in the Simulation Control, that should fix the issue.

Good luck and happy SimScaling!

Jousef


#9

Hi @jousefm

Thank you for your help; however, you got me a little confused when you said that 10,000 seconds was too much in your opinion but you still suggested increasing the maximum runtime.
Also, I did not explain myself too clear, I understand that it was not an error but more a suggestion that with all the different constants for turbulence that I was using, I got the exact same pattern in the initial 500s. The only one that is not convering under 1e-3 is pressure, would you by any chance know why is that ?

Sorry to bother you.
Thank you!
Carla


#10

Hi @cmartiso!

You have to make a difference between simulation time and run time. Usually one can use the Result Control Items to see if the forces converge to a constant value and we can say the solution to be converged when the values do not change anymore. I invite @Get_Barried and @vgon_alves here who might give you additional explanations.

In general you have many screws that you can turn in CFD in order to make a simulation converge. You can work on the initial conditions, relaxation factor, numerical schemes etc. But please be aware that a converged solution does not mean that the results you get are actually true. Some software packages normalize the convergence plots in such a manner so that they will always drop (or oscillate down to a specific value) just to comfort the user.

For the pressure you can start with the tolerances of 1e-5 or 1e-6 with a rel. tolerance of 0.01 and 0.001 respectively - that’s a bit of an experiment. @DaleKramer, guess you are the master of convergence studies now, can you give this user a tip here? :slight_smile:

Best,

Jousef


#11

Hi @cmartiso

I had a look at all your simulation ‘FORCES’ plots (in the post-processor tab > FORCES tree item ) and except for your very first run of your first simulation, all the force plots look very stable after about ~500 iterations (seconds or s).

I would reduce your ‘End time value [s]’ to say ~700 for this mesh for future runs on the mesh and then after the run, make sure that your forces are stable at that point. You can also try setting the ‘Absolute value’ for the residuals to stop it before 700s but that is likely not worth it.

No need to have a high End time value [s] when forces are stable at ~500s.

Set your ‘Maximum runtime [s]’ (which I think of as ‘Maximum realtime[s]’) to the max real time you want to let the run go to before it stops, in case it does not converge or reach the max iterations you set.

Your other option is to set very high End time value [s] and ‘Maximum runtime [s]’ , and then sit there and watch for convergence, both by low residuals and by obtaining stable forces, at which point just stop the simulation manually. If you so this, make sure you set maximum real time to <(3600*yourcorehrsleft/#coressimistouse). If you do not do this the simulation will appear stuck and not start and give you no error message. If this happens, just delete the stuck run and try a smaller max runtime that fits the formula above until it does start.

Simulation Runs will stop for mostly these 4 reasons;

  1. ALL Residuals have decreased to their individual ‘Absolute tolerance’ in ‘Numerics’ > ___ Residual Control > ‘Properties’. This is known as convergence.
  2. The run has reached the maximum iteration you set in ‘Simulation Control’ > ‘End time value [s]’, whether converged or not at this point.
  3. The real time of the run has reached the ‘Simulation Control’ > ‘Maximum runtime [s]’ that you set, whether converged or not at this point.
  4. The user stops the simulation manually.

In all those cases, the results should still get written and have a post-processor tab tree item created for them. (at least at the last write interval you have selected in each ‘Results Control Item’ > ‘Write Control’ > ‘Details’)

If you want to make sure that the mesh you use is giving you the highest accuracy you can expect, then you should do a Mesh Independence Study on it.

NOTE; I think the true test of convergence is whether your forces are stable and even then you can not be sure of their accuracy unless you are sure of your simulation setup and the Mesh independence of your mesh. AND then that accuracy should be confirmed with experimental results if possible (I know that somewhat defeats the purpose of CFD but as long as you don’t stray too far from examples that have proven to be close to experimental results, you can be somewhat confident in CFD results without having to compare to experimental results).

Hope that helps.

Dale


#12

Hi @jousefm and @DaleKramer,

Thank you both for taking the time to answer to my query and helping me out with your suggestions :slight_smile:
I understand your points and agree that even if my results converged to the criteria I wanted it would not mean that they are correct; where I would need experimental data.
I will proceed to decrease the end run time and increase the maximum run time.

Thank you again! :slight_smile:
Carla