|
[Sponsors] |
attachDetachFvMesh ignores uniformValue of attached patch (OpenFoam 1.5-dev) |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
October 27, 2010, 04:35 |
attachDetachFvMesh ignores uniformValue of attached patch (OpenFoam 1.5-dev)
|
#1 |
New Member
Patricia
Join Date: Oct 2010
Posts: 22
Rep Power: 15 |
Hello!
I submitted the following report to http://www.openfoam.com/mantisbt as suggested at the top of this forum. It was deleted without giving a reason. Are bugs related to the development version not accepted? Then the sticky post "Reporting OpenFOAM bugs" should say so. Still, could somebody please have a look at this issue: The following issue has been DELETED. ================================================== ==================== Reported By: schmittp54 Assigned To: ================================================== ==================== Project: OpenFOAM Issue ID: 68 Category: Bug Reproducibility: always Severity: major Priority: normal Status: new ================================================== ==================== Date Submitted: 2010-10-26 16:39 BST Last Modified: 2010-10-26 16:39 BST ================================================== ==================== Summary: attachDetachFvMesh ignores uniformValue of attached patch (OpenFoam 1.5-dev) Description: The attached case for OpenFoam 1.5-dev is a modified driven cavity. It attaches/detaches a barrier in the middle of the cavity with velocity U=(-1,0,0) at the barrier opposite to the moving wall. The simulation result (attached image) shows that instead of the given boundaryFields in 0/U: attachTop { type fixedValue; value uniform (-1 0 0); } attachBottom { type fixedValue; value uniform (-1 0 0); } the actual velocity on these patches is zero, when the barrier is attached. (We have confirmed this by printing the U.boundaryField() on the attached patch in a modified icoDyMFoam solver, which shows "value uniform(0,0,0);" instead of the expected "value uniform(-1,0,0);") Steps to Reproduce: Download and extract the attached newAttachDetach.tar.gz. Execute: cd newAttachDetach rm -rf 0.* 1* 2* 3* 4* 5* 6* 7* 8* 9* blockMesh faceSet setsToZones -noFlipMap icoDyMFoam Observe the velocity field U in paraFoam. ================================================== ==================== Issue History Date Modified Username Field Change ================================================== ==================== 2010-10-26 16:39 schmittp54 New Issue 2010-10-26 16:39 schmittp54 File Added: newAttachDetach.tar.gz 2010-10-26 16:49 henry Issue Deleted: 0000068 ================================================== ==================== |
|
October 29, 2010, 06:22 |
|
#2 |
New Member
Patricia
Join Date: Oct 2010
Posts: 22
Rep Power: 15 |
I'd appreciate some feedback, whether I am using attachDetachFvMesh in a wrong way, whether somebody did reproduce the problem and whether this is considered a bug by OpenFoam users who are more experienced than I am.
If this is confirmed as a bug I'll debug to the root of the problem and hopefully submit a patch. Thanks Patricia |
|
October 31, 2010, 03:02 |
|
#3 |
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,905
Rep Power: 33 |
I already wrote a rude answer about OpenCFD deleting bug reports etc, but let's not bother with that: it is clear that the open forum bug tracker is needed. Please carry on reporting your bugs here for the moment; a further announcement will follow.
Now, to attach/detach: when the geometry is connected, the patches will disappear into nothing, and when disconnected they will jump to existence from zero size. Therefore, there is nothing for me to map from. The correct boundary condition for your case is uniformFixedValue, which will work correctly. Enjoy, Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk |
|
November 1, 2010, 04:04 |
|
#4 |
New Member
Patricia
Join Date: Oct 2010
Posts: 22
Rep Power: 15 |
Thanks a lot, Hrv.
Using uniformFixedValue instead of fixedValue solved the problem. Patricia |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Superlinear speedup in OpenFOAM 13 | msrinath80 | OpenFOAM Running, Solving & CFD | 18 | March 3, 2015 05:36 |
OpenFOAM 1.5 dev | LVDH | OpenFOAM | 98 | May 5, 2010 17:01 |
CheckMeshbs errors | ivanyao | OpenFOAM Running, Solving & CFD | 2 | March 11, 2009 02:34 |
[Gmsh] Import gmsh msh to Foam | adorean | OpenFOAM Meshing & Mesh Conversion | 24 | April 27, 2005 08:19 |
Multicomponent fluid | Andrea | CFX | 2 | October 11, 2004 05:12 |