Different dimensions for dimensions Issue in FSI when turbulence model is used - OpenFOAM adapter #158
Comments
|
This issue has been mentioned on preCICE Forum on Discourse. There might be relevant details there: https://precice.discourse.group/t/different-dimensions-for-dimensions-issue/535/6 |
|
I cannot reproduce this issue with OpenFOAM v2012 and since I have at the moment no foundation version installed I cannot try with another OpenFOAM version. Are you tied to use OpenFOAM v7? |
|
Yes, I use OpenFOAM v7. |
|
I'm having the same issue with OpenFOAM v7 and kOmegaSST for turbolence. I also tried with kOmega and I get MPI_ERR_TRUNCATE. There are any news for fixing the dimensions error for kOmegaSST? |
|
I am having the same issue with OF10 and Calculix using kOmegaSST turbulence model. Is there any news regarding this? |
|
If I understand correctly, this seems to be specific to the Foundation versions. As I wrote in the preCICE forum, I would assume that the |
|
Another user reported that with OpenFOAM v2212:
In any case, this only affects checkpointing, i.e., only implicit coupling (explicit should work with any turbulence model). This is only a software issue, which we don't yet understand. |
|
Yes i have the same exact issue with komega sst on OpenFOAM v2312 |
|
Hello @MakisH I still have the same problem with the K-omega sst and the OpenFOAM adapter, did you manage to figure out where is the issue, please? |
|
Hi! No, we have not yet looked into it. It is clear that we need to fix it, it is near the top of the list, but we currently have other priorities. Any clues or contributions in this direction are welcome! 🤗 |
|
@KariimAhmed let's look into this together. I think that, by fixing this, we will fix more strange issues. But first, I need to be able to reproduce it. I modified our |
|
This issue has been mentioned on preCICE Forum on Discourse. There might be relevant details there: https://precice.discourse.group/t/fsi-openfoam-my-solver-using-python/1823/2 |
|
@MakisH Thanks for considering this issue, the problem is triggered with me when I use the K-omega sst with my flapping foil with FSI. Also when using k-omega it simulates some time steps then it diverges and crashes, only the laminar is working fine. Concerning the case you mentioned I don't know exactly how can the issue be triggered, I saw that people are reporting this issue when using turbulent models in different cases but we don't know why this happens. |
|
It is clear that this issue happens to user's cases, but if I don't have a failing example at hand, it is very challenging for me to fix the problem. |
|
This issue has been mentioned on preCICE Forum on Discourse. There might be relevant details there: https://precice.discourse.group/t/openfoam-ras-models/2047/2 |
|
I am running an overset-OpenFOAM coupled with calculix using K-omegaSST turbulence model and after the first time step i faced this error |
Hi makis, I have made a case related to this problem, you may run this case to catch the error. |
|
Hey guys, I have a student that states that eliminating the cache of grad(U) from the fvSolution dictionary solves the problem. Well, we didn't dig into this but I just wanted to let you know this because it may help you tracing the root cause. |
Unfortunately, I never used the cache of grad(U) and I have the same problem |
|
@KariimAhmed we now have a student looking into this, but we cannot give a timeline at the moment. Thanks a lot for following up on this and for uploading cases and helpful details. |
|
Hi all, I am the student that Makis mentioned. First of all, thank you, Charlie (@c7888026), for providing the failing case, which helped with debugging the issue. I've found a workaround you can use for now, but I will try to submit a bugfix pull request ASAP. The error occurs with the preCICE implicit coupling method, which stores past timesteps of fields called checkpoints. Also, it occurs with the Somehow the A possible solution is to call WorkaroundFor the time being, I will post a workaround. The workaround is to run the OpenFOAM case until the first timestep is written, and then restart the case from that timestep. You need to change the FoamFile
{
version 2.0;
format ascii;
class dictionary;
object controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
application pimpleFoam;
startFrom startTime;
startTime 5e-6; // Restart from 1st timestep
stopAt endTime;
endTime 1;
deltaT 5e-6;
writeControl adjustable;
writeInterval 5e-6; |
|
Hi Daniels, Thanks very much for posting. Your workaround appears to be consistent which what we have seen. I normally initialize the flow with a transient simulation, and then run the FSI reading the last converged solution and kOmegaSST is not giving any problem. We never realized that this was the reason why the case was running succesfully. |
|
Hello @vidulejs , Courant Number mean: 0.0145696 max: 1.93691 DICPCG: Solving for cellDisplacementx, Initial residual = 1, Final residual = 9.47425e-07, No Iterations 287 [3] ============= Interestingly, When I ran the same simulation in serial ( no mpirun ) just one core for OpenFOAM ( parallel implicit for precice) it ran fines for the K-omega-SST, I can send you the test case if you want. |
|
Hi @KariimAhmed, Thanks for the information. Could you provide a test case and/or full log? Your error seems to be different than the one I observed. Did you get a 'Different dimensions' error? |
|
The log is attached above , I found that the variable yPSi that is calculated in the fvSolution and required by the method of the wall distance in the fvSchemes is the problem, so it behaves as the gradU as you described and not passed correctly through the check point . I changed the wallDist method to meshWave as @c7888026 did in his case , and it worked fine even with K-omega sst and in parallel setting using mpirun , so it is matter of variables that are not passing well ( may be ) through the checkpoint step. |
|
@KariimAhmed we already discussed that this would probably also hit function objects creating objects later on. This is useful feedback, because it means that the fix we were planning will not solve this case. Thank you! @vidulejs we then really need to change the way we store checkpoints, not change the time |
|
The fix for this is now merged in develop. Everyone affected, please test and let us know here. A bugfix release will follow. |
Hi there,
This issue was found when I was doing a FSI simulation using OpenFOAM v7 / CalculiX v2.15 / preCICE v2.0.0.
Please let me lead you to this discourse-post for more details.
As suggested by @MakisH , a brief introduction to the settings of turbulence model in OpenFOAM is to simply turn on the turbulence by setting
/constant/turbulencePropertiesfile, using:Of course, the corresponding initial conditions such as
k,omega,nut,pandUare well defined in the0/directory.When the turbulence model is turned on, the FSI simulation stops at the 2nd iteration of the first time step of the coupling (shown in the figure in the post)
Interestingly however, when I turned off the turbulence (switch to
laminar):simulationType laminar;The FSI simulation went well and no errors are reported. However, the results are definitely not I'm expecting since the turbulent behaviours cannot be well resolved in my FSI simulation.
As @MakisH said, I do also suspect this issue might be originated from the OpenFOAM adapter side, so I'm looking for help from developers.
Should you requires more information please contact me directly and I'm happy to assists.
The text was updated successfully, but these errors were encountered: