CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Bugs (http://www.cfd-online.com/Forums/openfoam-bugs/)
-   -   attachDetachFvMesh ignores uniformValue of attached patch (OpenFoam 1.5-dev) (http://www.cfd-online.com/Forums/openfoam-bugs/81439-attachdetachfvmesh-ignores-uniformvalue-attached-patch-openfoam-1-5-dev.html)

schmittp54 October 27, 2010 05:35

attachDetachFvMesh ignores uniformValue of attached patch (OpenFoam 1.5-dev)
 
2 Attachment(s)
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
================================================== ====================

schmittp54 October 29, 2010 07:22

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

hjasak October 31, 2010 05:02

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

schmittp54 November 1, 2010 06:04

Thanks a lot, Hrv.
Using uniformFixedValue instead of fixedValue solved the problem.

Patricia


All times are GMT -4. The time now is 05:47.