|
[Sponsors] |
[Other] How can the defualt checkMesh criteria on openfoam be changed? |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
January 19, 2017, 05:15 |
How can the defualt checkMesh criteria on openfoam be changed?
|
#1 |
New Member
Anonymous
Join Date: Jan 2017
Location: India
Posts: 3
Rep Power: 9 |
Hi All,
I am trying to simulate the flow through a butterfly valve on openFoam. I have created two different meshes (fine and coarse) with 8.6 million and 3.11 million mesh count. Both the meshes looks fine and does not show any errors in checkMesh operation. Though no error has been detected the solution diverges in 10 iterations for the coarse mesh while it converges in 400 iterations for fine mesh. The only difference I find in both the meshes is that the non-orthogonal angle for coarse mesh is higher as compared to that of fine mesh (please refer the attached image for comparison). Now my question is: Can we change the default checkMesh criteria in openfoam for non-orthogonal faces from 70 degree to 60 degree or any other angle? Alternatively How can I write a vtk file for non-orthogonal faces with an angle more than 60 degree? Thanks for help. |
|
January 23, 2017, 06:53 |
|
#2 |
Senior Member
Join Date: Mar 2010
Location: Germany
Posts: 154
Rep Power: 16 |
Hi,
mesh quality criteria are usually specified in system/meshQualityDict. The path to such dictionary files can be passed to checkMesh by using the -meshQuality option. Please have a look at the following links to obtain more insight: https://github.com/OpenFOAM/OpenFOAM...sh/checkMesh.C https://github.com/OpenFOAM/OpenFOAM...ualityDict.cfg (default settings) Cutter |
|
January 24, 2017, 06:13 |
|
#3 |
New Member
Anonymous
Join Date: Jan 2017
Location: India
Posts: 3
Rep Power: 9 |
Dear Mr Cutter,
Thank you for the reply. I have tried to run the meshQualityDict with the required mesh quality parameter and it worked. But now when i write the vtk file for the defined mesh criteria through foamtoVTK -faceSet meshQualityFaces it writes all the faces in the meshQualityFaces. Is there any way to write a separate vtk file for every user defined checkMesh criteria? Like i wanted to write vtk files for user defined maxNonOrtho and user defined maxBoundarySkewness separately. Thanking in anticipation. |
|
January 24, 2017, 06:20 |
|
#4 |
New Member
Anonymous
Join Date: Jan 2017
Location: India
Posts: 3
Rep Power: 9 |
Please reply as per your earliest convenience.
Best Regards |
|
February 2, 2017, 22:05 |
|
#5 |
Senior Member
Join Date: Aug 2013
Posts: 407
Rep Power: 15 |
Hi,
Doesn't the output of checkMesh go to individual "sets"? nonOrthoFaces would be one, skewFaces would be another etc. etc. In which case you can create each set separately with the foamToVTK command, no? Cheers, Antimony |
|
September 24, 2019, 12:04 |
|
#6 |
Senior Member
Join Date: Sep 2017
Posts: 246
Rep Power: 11 |
This is an old thread, but it shows up on a Google search, so here is what I have found:
You can get checkMesh to automatically convert sets to vtk format for viewing using Code:
checkMesh -meshQuality -writesets vtk The -meshQuality option in that command causes a separate check based on ./system/meshQualityDict. Faces that fail *any* of those user-defined criteria are all exported into *one* set: ./postProcessing/constant/meshQualityFaces/meshQualityFaces.vtk. The standard sets (skewFaces and so on) are based on the standard criteria. So, it appears that there is no way to get a separate VTK for each *user-defined* criterion. If you want to look only at, for example, skewness > 7, then you need to hack your ./system/meshQualityDict such that all faces pass all the other criteria. (Save a copy of a sensible meshQualityDict, for use in meshing!) For example, you might find it necessary to set Code:
minTetQuality -9.999e30; |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Getting Started with OpenFOAM | wyldckat | OpenFOAM | 25 | August 14, 2022 13:55 |
[OpenFOAM.org] A Mac OS X of23x Development Environment Using Docker | rt08 | OpenFOAM Installation | 1 | February 28, 2016 19:00 |
OpenFOAM v3.0.1 Training, London, Houston, Berlin, Jan-Mar 2016 | cfd.direct | OpenFOAM Announcements from Other Sources | 0 | January 5, 2016 03:18 |
Modified OpenFOAM Forum Structure and New Mailing-List | pete | Site News & Announcements | 0 | June 29, 2009 05:56 |
Adventure of fisrst openfoam installation on Ubuntu 710 | jussi | OpenFOAM Installation | 0 | April 24, 2008 14:25 |