CFD Online Logo CFD Online URL
Home > Forums > Software User Forums > SU2

Issues while simulating a 3D unsteady case

Register Blogs Members List Search Today's Posts Mark Forums Read

LinkBack Thread Tools Search this Thread Display Modes
Old   March 18, 2021, 14:55
Default Issues while simulating a 3D unsteady case
New Member
Join Date: Nov 2019
Location: Poland
Posts: 13
Rep Power: 6
IwantTobeGood is on a distinguished road
Hello. I am dealing with an issue that I can't solve by myself.

I am trying to simulate a 3D case of fluidic pinball - the file I am working on now has no rotation on any cylinder. I have gone through some tutorials that were on the SU2 page, and did some of my own cases, but all of them were in 2D, plus this is the first time I am doing an unsteady case myself. While trying to simulate the case, I ran into multiple issues.

1) I can't seem to find the option to increase the iterations per time step. One post from 2015 showed that in earlier version there was a variable named EXIT_ITER, which controlled that, but in 7.0.7 I don't see any similar variable. While doing a steady simulation I get inner iterations counted down normally, I either see inner iteration 0 or no listed iterations at all for each time step. I have attached a picture that shows an example of what I mean. I did tinker with "Writing frequency for screen output" settings, but those did not help. Does that mean that by controlling the size of the time step I control the accuracy of the result?

2) I can't get the solver to converge - it always reaches the time/iteration limit and then for some reason crashes on post processing, resulting in bogus results. I have already moved from FGMRES linear solver to BCGSTAB due to multiple instances of linear solver diverging or SU2 diverging. For convective numerical method I use Lax-Friedrich, but I am also giving Roe a spin right now to see if it works. I had some issues with JST. I have also canged Hybrid Parallel (MPI+OpenMP) options since I use parallel computation to run the simulation. I also disabled MUSCL_FLOW, LOW_MACH_CORR and LOW_MACH_PREC, reduced CFL number from 40 to 10, I think that is all of what I changed. The most I ran the solver for was 4500 time steps, but I assume I need to run the simulation for a longer time? Or is it also a case of a mistake in my code? From what I understand resutls when the convergence is not achieved may be incomplete?

3) If I want to use the restart function properly, should I first make a steady state simulation first and restart or can I run an unsteady simulation first, and then run it again with restart on? I have seen some people suggesting doing the former in a case of unsteady simulation, but I couldn't find a lot of information on the topic, and while browsing the post on this site I have found little regarding my issue.

4) I would also like to ask if I can name multiple centres of rotation for mltiple MOVING_WALL markers, for instance for 2 cylinders with different centres? Or if I want to do multiple rotating cylinders I need to use separate config files?

Due to the fact that I made small elements while meshing, the mesh file was too big to attach, therefore I added only the .geo file for Gmsh, alongside my config file.

Thank you in advance for any responses.
IwantTobeGood is offline   Reply With Quote

Old   March 19, 2021, 06:31
Join Date: May 2017
Posts: 31
Rep Power: 8
raviramesh10 is on a distinguished road
Hello Hubert,

This is a nice case that you are currently working on. Here are the answers to your questions from my knowledge:

1. The iterations option depends on whether you would like to increase the number of inner or outer iterations for your unsteady simulation. For the inner iterations, there is an option called INNER_ITER under the TIME DEPENDENT SIMULATION settings, and for the outer iterations, it is called TIME_ITER under the heading of COMMON PARAMETERS to define the numerical method. EXIT_ITER has been depreciated as far as I know, we are currently using version 7.1.1.

And "Writing frequency for screen output" simply means that your solution will be written for each iteration and shown in the screen that an output file is being written (either vtk or vtu).

And whether your time step controls the accuracy of your solution depends on your physical problem itself. Do you know what CFL number you are planning to use? And also the vortex shedding frequency? Maybe it would be good to think along those lines and find your time step accordingly. Based on that, it will affect the accuracy of your result.

2. Indeed, the FGMRES solver is quite useful as it takes the regular minimum residual algorithm into account. You could try using different slope limiter, possibly? That would ensure that your solution is monotonic within your grid, while being differentiable. Venkatakrishnan is pretty good for structured grids from what I have seen in the literature, maybe you could try to use that (if you are using a structured one, that is). My suggestion would be to start from JST and then try a low dissipation scheme like Roe or AUSM.

You will have to check the trends of certain important parameters. Did you check your C_{l} and C_{d} plots? That should give you an idea of whether it is proceeding towards a steady state solution. The residuals will most likely be fluctuating depending on your flow physics, and might not necessarily provide a good idea about your convergence.

3. You can definitely start an unsteady simulation from the beginning by specifying the RESTART_ITER option under the TIME DEPENDENT SIMULATION settings. Whether you want to feed your steady simulation to start the unsteady one depends on your flow physics again. Do you think that your numerical scheme would fall out if you started your unsteady problem again? If yes, try using a converged steady state solution first. If not, try starting from where you stopped.

4. Yes, that should be possible if you specify the coordinates of the different centres under MOVING_WALL. This has been done for tandem cylinders in the past, you might want to check the configuration file for that out once (and yes, from my knowledge, one .cfg file was sufficient in that case).

Hope my answer provides a direction to start again.
raviramesh10 is offline   Reply With Quote

Old   March 22, 2021, 07:01
New Member
Join Date: Nov 2019
Location: Poland
Posts: 13
Rep Power: 6
IwantTobeGood is on a distinguished road
Thank you for your reply Ravi. It has given me a few ideas that guided me in the right direction.

Also, I just realized that for some reason the first post did not have attached files, so I am attaching them once again, updated.

1) I managed to manipulate with the number of iteration per time step, now I need to run a test with a relatively big number of iterations and time steps to see if the solver converges.

2) I noticed that I used Venkatakrishnan-Wang slope limiter, changing it back to Venkatakrishnan made the simulation more stable for me. As my numerical method, I used Lax-Friedrich and it seemed to calculate just fine, although I will confirm it later by checking the history file and the results the solver yields, since I had some issues with the history file before (I could not select a column with results, for some reason it seemed like they were just floating about, not pinned to any cell). At the very least there is no divergence issues anymore.

3) Regarding the last 2 points, I have yet to try to use restart with both steady and unsteady results, since I just now got the simulation to run properly, and the multiple rotation centres, since I am still stuck on a test case with no rotation to see if everything else works. Once I confirm everything else is fine and move to the cases with rotation, I will give my feedback on those, if necessary.

Thank you once again for the tips, they were really helpful and gave me a few ideas as to what to look into.
Attached Files
File Type: txt pinballtest.txt (705 Bytes, 5 views)
File Type: txt Setup_mastertest_0.txt (25.7 KB, 5 views)
IwantTobeGood is offline   Reply With Quote


convergence, moving wall, restart file, time stepping, unsteady flow

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On

Similar Threads
Thread Thread Starter Forum Replies Last Post
Test Case CFL Number Issues with Software Update JBCFD SU2 3 July 14, 2017 12:05
[waves2Foam] Error in simulating wave breaking case Sujatha OpenFOAM Community Contributions 0 March 16, 2014 06:06
How to calculate time average variable in Unsteady case lehoanganh07 FLUENT 1 March 13, 2014 04:44
unsteady case, how to update the porosity? ylw2010 Fluent UDF and Scheme Programming 0 May 3, 2012 23:36
how to get mean variables corectly for unsteady case aoun FLUENT 0 January 31, 2012 16:40

All times are GMT -4. The time now is 12:17.