Splitting the mesh for AMI
1 Attachment(s)
Hey Everybody!
I am working for a while now with OpenFoam and like the solver a lot. There is however a problem which keeps repeating it self, and I can't figure out what I am doing wrong. I try to simulate a rotating wing using the AMI interface (I deliberately did not choose for SRF or MRF for now). I make my mesh as shown in the propellor case using this as my snappyHexMeshDict: Code:
/*--------------------------------*- C++ -*----------------------------------*\ Code:
/*--------------------------------*- C++ -*----------------------------------*\ The problem is now that when I rotate my mesh the inner AMI (AMI2) has points in the outer AMI creating stretched cells (as shown in the attached image). Does anybody know where I went wrong? I am using OpenFoam 3.0x by the way. Thank you in advance! |
Greetings Wouter,
I've got the feeling that this is a bug in OpenFOAM or that something went wrong in the mesh generation step. Can you please share the case you have, but without the wing inside it, so that I or anyone else can test it more easily? Best regards, Bruno |
1 Attachment(s)
Hey wyldckat
I have solved the problem by meshing the inner and the outer part separate and using mergmesh to merge both meshes. So I think the problem lies complete in the meshing part. I have added my case files to this post. I hope it helps! I have used a cylinder in this case since the sphere is to big for the upload! Wouter |
Hi Wouter,
Many thanks for the test case! Can you please tell me which commit you're using from 3.0.x? To see which one it is, run the following commands: Code:
foam Best regards, Bruno |
Hey Bruno,
I have not installed it using git, so I don't get a response from git. I have followed the instructions listed here : http://www.openfoam.org/download/ubuntu.php I have installed it at least 3 weeks ago. So no recent update. Wouter PS Thank you for implementing this in the code! It is really an awsome feature. |
Hi Wouter,
Quote:
Quote:
The bad commit is related to this comment and respective patch: http://www.openfoam.org/mantisbt/view.php?id=1479#c5493 - namely the patch was integrated in this commit: https://github.com/OpenFOAM/OpenFOAM...33942e88f3a855 It was reverted a few days later and recently I managed to figure out the proper fix (or at least I hope so), which is already in the latest 3.0.x. If you only get the problem with the sphere, please provide the case without the wing and sphere geometries and let me know the centre and radius of the sphere, so that I will create a new one with ParaView. Best regards, Bruno |
1 Attachment(s)
Hey Bruno,
I am indeed using 3.0.0. If I use the command: Code:
moveDynamicMesh -checkAMI Code:
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Wouter |
Hi Wouter,
OK, now I'm really worried. I got this instead: Code:
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // I ran the case with the following commands: Code:
blockMesh Code:
stopAt nextWrite; Because my suspicion is regarding a possible problem with a specific build... which once in a while happens due to a compiler flaw/bug. Best regards, Bruno |
Hey Bruno,
Where do I find the exact build number? I am running it on Ubuntu 15.10. I have tested it on two different computers both running Ubuntu 15.10, both giving the exact same problems. I am running the same commands as your are running, except I am running: Code:
decomposePar Thank you for all your help! Wouter |
Hi Wouter,
Quote:
The exact version is given by any application that is executed from OpenFOAM. For example: Code:
blockMesh -help Code:
Using: OpenFOAM-3.0.0 (see www.OpenFOAM.org) Quote:
Oh, definitely... Wow! OK, I managed to reproduce the error with the steps you've pointed out! Now, let me see if OpenFOAM-3.0.x does it better... nope. Same problem. OK, I've ran with the latest OpenFOAM-history - https://github.com/OpenCFD/OpenFOAM-history - and it didn't give me any problems for the same situations that would break when using 3.0.0 and 3.0.x. So my question to you now is this: Can we use this test case for reporting this issue on the bug tracker? Because this means that the missing code has to be ported from OpenFOAM-history to OpenFOAM-dev/3.0.x and I/we can use this case for testing if things work as intended. Best regards, Bruno |
Hey Bruno,
I am sort of happy that you've gotten the same error. Are the steps wrong that I took? My build number is: Code:
Using: OpenFOAM-3.0.0 (see www.OpenFOAM.org) Wouter |
Hi Wouter,
Quote:
The workaround until the bug is fixed is for you to mesh in serial mode instead of parallel mode. In other words, to use the same commands I did. Quote:
Quote:
Please provide as much information as possible (related to reproducing the bug), along with the test case. Add a link to this thread only as a fallback, in case you feel like you might have missed some details. I'll come by the bug tracker as soon as I can, in case you miss any details and to add more details as I find more about this issue. Best regards, Bruno |
hey Bruno,
I will add this bug to the bug tracker. The problem is also found when meshing in serial (not in this case, but in other cases it was irrelevant if I used serial or parallel compuation). Thank you for your help! Wouter |
Hi Wouter,
Many thanks for reporting this! I see you reported it here: http://www.openfoam.org/mantisbt/view.php?id=1936 I'll try to take a look into this starting today and in the next couple of days. Nonetheless, in the meantime, can you please also provide the test case that fails when running in serial mode? Best regards, Bruno |
Hey Bruno,
This week is very busy at work, I hope to give you a case which fails this weekend! I will share it through dropbox, since the forum upload is to small. Wouter |
Hi Wouter,
Quote:
The forum has a limit of 200kB. If the package is 2MB or less, I believe the bug tracker can handle it. Best regards, Bruno |
Thank you both, nice discussion. It helped me to settle the case.
|
no parallel for SnappyHexMesh
Meshing with snappy one one processor solved my problem of AMI weight going to zero.
This bug has to be reported |
All times are GMT -4. The time now is 05:24. |