CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Bugs

attachDetachFvMesh ignores uniformValue of attached patch (OpenFoam 1.5-dev)

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 27, 2010, 04:35
Default attachDetachFvMesh ignores uniformValue of attached patch (OpenFoam 1.5-dev)
  #1
New Member
 
Patricia
Join Date: Oct 2010
Posts: 22
Rep Power: 6
schmittp54 is on a distinguished road
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
================================================== ====================
Attached Images
File Type: png barrier.png (13.1 KB, 6 views)
Attached Files
File Type: gz newAttachDetach.tar.gz (2.2 KB, 5 views)
schmittp54 is offline   Reply With Quote

Old   October 29, 2010, 06:22
Default
  #2
New Member
 
Patricia
Join Date: Oct 2010
Posts: 22
Rep Power: 6
schmittp54 is on a distinguished road
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
schmittp54 is offline   Reply With Quote

Old   October 31, 2010, 04:02
Default
  #3
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,741
Rep Power: 20
hjasak will become famous soon enough
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
hjasak is offline   Reply With Quote

Old   November 1, 2010, 05:04
Default
  #4
New Member
 
Patricia
Join Date: Oct 2010
Posts: 22
Rep Power: 6
schmittp54 is on a distinguished road
Thanks a lot, Hrv.
Using uniformFixedValue instead of fixedValue solved the problem.

Patricia
schmittp54 is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
OpenFOAM 1.5 dev LVDH OpenFOAM 98 May 5, 2010 17:01
Superlinear speedup in OpenFOAM 13 msrinath80 OpenFOAM Running, Solving & CFD 17 August 22, 2009 03:59
CheckMeshbs errors ivanyao OpenFOAM Running, Solving & CFD 2 March 11, 2009 03:34
Import gmsh msh to Foam adorean Open Source Meshers: Gmsh, Netgen, CGNS, ... 24 April 27, 2005 08:19
Multicomponent fluid Andrea CFX 2 October 11, 2004 05:12


All times are GMT -4. The time now is 02:24.