|
[Sponsors] |
[cfMesh] How do we perform edge refinement in cfMesh |
![]() |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
![]() |
![]() |
#1 |
New Member
Dion
Join Date: Dec 2014
Location: Bremen, Germany
Posts: 13
Rep Power: 11 ![]() |
Hello everyone,
I started using cfMesh for the past few days. I find it very useful and with some difficulties. For exemple i want to use the edgeMehRefinement dictionary option. I uses V1.1.1 currently. I tried to follw the user guide and i didnt find any solution. For exemple i tried to extract the edge Features using surfaceFeatureEdges utility and save it in .vtk format. When i try to insert this file in my dictionary i get a error like Code:
----> Foam Fatal Error unknown file extension vtk valid types are : 5 ( bdf eMesh inp nas obj ) ... Code:
---> FOam Fatal Error: Expected a '(' while reading VectorSpace>Form. Cmpt, nCmpt>, foulnd on line22 an error with regards, Dinesh |
|
![]() |
![]() |
![]() |
![]() |
#2 | ||
Senior Member
|
Hi,
An example for edgeMeshRefinement looks like this: edgeMeshRefinement { edge1 { edgeMesh "edges.vtk"; cellSize 0.005; refinementThickness 0.002; } edge2 { edgeMesh "edge2.vtk; additionalRefinementLevels 2; } } The edgeMesh keyword is the name of the file relative to the directory of the case. cellSize is the desired cell size, and the selected value is the first multiplier of maxCellSize that is smaller than cellSize. additionalRefinementLevels specifies the desired number of refinement levels relative to maxCellSize. refinementThickness is the distance from the edge where the refinement still applies. Quote:
surfaceFeatureEdges <inputSurface> <surfaceWithFeatureEdges> -angle 40 generates a new surface mesh with selected feature edges or additional patches. Feature edges are stored when you export into fms files, and in other cases the utility generates patches whose boundaries correspond to the detected feature edges. To extract the edge mesh from the fms file, you can FMSToSurface as follows: FMSToSurface <surfaceMesh> <outputSurfaceMesh> -exportFeatureEdges Alternatively, you can extract edges that you want to use for refinement in Paraview and save them is a vtk file. Quote:
In addition, what version of OpenFOAM are you using? I have observed problems reading edge meshes with foam-extend. Regards, Franjo
__________________
Principal Developer of cfMesh and CF-MESH+ www.cfmesh.com Social media: LinkedIn, Twitter, YouTube, Facebook, Pinterest, Instagram |
|||
![]() |
![]() |
![]() |
![]() |
#3 |
New Member
Dion
Join Date: Dec 2014
Location: Bremen, Germany
Posts: 13
Rep Power: 11 ![]() |
Hello Franjo,
Thank you very much for your reply. As you have mentioned in your post. Code:
edgeMeshRefinement { edge1 { edgeMesh "edges.vtk"; cellSize 0.005; refinementThickness 0.002; } edge2 { edgeMesh "edge2.vtk; additionalRefinementLevels 2; } } Code:
----> Foam Fatal Error unknown file extension vtk valid types are : 5 ( bdf eMesh inp nas obj ) Code:
In addition, what version of OpenFOAM are you using? I have observed problems reading edge meshes with foam-extend. with regards, Dinesh |
|
![]() |
![]() |
![]() |
![]() |
#4 |
New Member
Dion
Join Date: Dec 2014
Location: Bremen, Germany
Posts: 13
Rep Power: 11 ![]() |
Hello Mr. Franjo,
I tried with a standard OF v2.3.0 and the problem relating the edgeFile is now solved. I can now able to use the edgeRefinement without any problem. Thank you for your effort. with regards, Dinesh Nithyanandham |
|
![]() |
![]() |
![]() |
![]() |
#5 |
Senior Member
|
It was my pleasure to help and please let us know if you run into any other difficulites with cfMesh.
Kind regards, Franjo
__________________
Principal Developer of cfMesh and CF-MESH+ www.cfmesh.com Social media: LinkedIn, Twitter, YouTube, Facebook, Pinterest, Instagram |
|
![]() |
![]() |
![]() |
![]() |
#6 |
New Member
Jiri Stejskal
Join Date: May 2014
Posts: 5
Rep Power: 12 ![]() |
Dear Franjo,
I would also like to test the edge refinement in cfMesh. I extracted the edges as you described earlier using surfaceFeatureEdges and then FMSToSurface. When running cartesianMesh I get the following error: --> FOAM FATAL IO ERROR: incorrect first token, expected <int> or '(', found on line 1 the word '#' file: trailingEdgeWall_featureEdges.vtk at line 1. From function operator>>(Istream&, List<T>&) in file /nfs/CFDWRK/bigdisk/SOFTWARE/foam/foam-extend-3.1/src/foam/lnInclude/ListIO.C at line 149. FOAM exiting I attach the .vtk file generated by FMSToSurface I'm using for your reference (renamed to .txt to be able to upload it here). Do you have any idea what I'm doing wrong? Thank you. |
|
![]() |
![]() |
![]() |
![]() |
#7 | |
Senior Member
|
Hello,
Quote:
__________________
Principal Developer of cfMesh and CF-MESH+ www.cfmesh.com Social media: LinkedIn, Twitter, YouTube, Facebook, Pinterest, Instagram |
||
![]() |
![]() |
![]() |
![]() |
#8 |
New Member
Jiri Stejskal
Join Date: May 2014
Posts: 5
Rep Power: 12 ![]() |
Dear Franjo,
Thank you for your response, I'll try it out with OpenFOAM... |
|
![]() |
![]() |
![]() |
![]() |
#9 |
Member
Ali
Join Date: Oct 2013
Location: Scotland
Posts: 66
Rep Power: 12 ![]() |
Hi Folks
I've been modelling a submerged jet impingement test with cfMesh with fairly good results (especially for the ease of use etc.) One issue I am having is that in one of my geometries, the edge of the pipe, or the edge of the mesh is being 'cut' by the mesher. Does anyone have any ideas? I tried the above method of exporting the edges as .vtks, but that never worked. My meshing process is as follows: 1. Create fluid geometry in Autodesk Inventor 2. Import .step file from inventor to Salome 3. Export surfaces from Salome to .stls 4. Merge .stls into one 'master' .stl 5. Mesh with cfMesh: using 'cartesianMesh' (using of4x) Attached are some images of the problem. The settings are the same for both meshes, (although the images show a finer mesh around the nozzle in the cone mesh) however the mesh with the cone in it has curved edges at the pipe exit. Does anyone have any suggestions? ![]() ![]() ![]() ![]() |
|
![]() |
![]() |
![]() |
![]() |
#10 |
Member
Ali
Join Date: Oct 2013
Location: Scotland
Posts: 66
Rep Power: 12 ![]() |
Hi Folks
I managed to solve the problem by doing: surfaceFeatureEdges constant/triSurface/master.stl master1.stl Where master.stl was my original .stl, and master1.stl is the new one to be meshed. Cheers |
|
![]() |
![]() |
![]() |
![]() |
#11 |
Senior Member
Charles
Join Date: Aug 2016
Location: Vancouver, Canada
Posts: 150
Rep Power: 10 ![]() |
Just a note here: meshDict keyword edgeMesh is changed to edgeFile in version 1.1.
__________________
Charles L. |
|
![]() |
![]() |
![]() |
Tags |
cfmesh, edgerefinement |
|
|
![]() |
||||
Thread | Thread Starter | Forum | Replies | Last Post |
[snappyHexMesh] SnappyHexMesh running killed! | Mark JIN | OpenFOAM Meshing & Mesh Conversion | 7 | June 14, 2022 01:37 |
how to set periodic boundary conditions | Ganesh | FLUENT | 15 | November 18, 2020 06:09 |
killed "snappyHexMesh" | parkh32 | OpenFOAM Pre-Processing | 2 | April 8, 2012 17:12 |
[snappyHexMesh] snappyHexMesh aborting | Tobi | OpenFOAM Meshing & Mesh Conversion | 0 | November 10, 2010 03:23 |
fluent add additional zones for the mesh file | SSL | FLUENT | 2 | January 26, 2008 11:55 |