CFD Online Logo CFD Online URL
Home > Forums > Software User Forums > ANSYS > CFX


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

LinkBack Thread Tools Search this Thread Display Modes
Old   April 23, 2008, 11:26
Francesco - University of Florence, Italy
Posts: n/a
Hi all!

I've created a mesh and i've done a check of my mesh.

The "check" found various error like:

"multiple edge" "penetrating elements" "single edge" "surface orientation" "stuck elements"

How can i do to resolve this error? Is there a procedure, a specific command or i have to modify le geometry?



  Reply With Quote

Old   April 23, 2008, 12:00
Default Re: MESH ERROR
Posts: n/a
From the problems you have listed, my best guess is you ran Prism on a poor quality mesh. Ensure that your elements are small enough that there are at least 2 elements in every gap.

Single and multiple edge elements are not always errors. If you have an internal wall that has not been split, the edges in contact with external walls and the internal wall will be multiple edges and the edges within the fluid region on the internal wall will be single edges.

If you do not have an internal wall then these indicate a problem with the topology of your geometry. Single edges likely indicate holes in the mesh (if they form a closed loop). Holes in the mesh can be caused by element sizes too large to represent the geometry, or missing surfaces. Fix the geometry before trying to mesh it. Also, be sure you "build topology" after making any changes.

Surface orientation errors indicate overlapping cells. I know of no way to repair this other than remeshing the region around the overlapping cells. This error is frequently created by ICEM CFD's Prism mesher if the input mesh is of poor quality. Be sure to smooth your volume mesh before running prism. In the smoother set the volume elements to float and the surface elements to smooth, enable laplacian smoothing. Keep smoothing until your worst triangle quality is above 0.3. Once that's done, disable laplacian smoothing and freeze the surface elements. Now smooth the volume elements until the worst quality is about 0.3.

When running Prism, you should set the global prism parameters so that it only creates 1 prism layer. You can change the smoothing options there as well to 0 surface smoothing steps and 1 volume smoothing step, since you did the smoothing manually. (Prism will not run if volume smoothing steps is set to 0.) The thickness of that layer should be the total thickness of all the desired layers.

After prism runs, go back to the smoothing tool. Freeze the surface elements (quad, tri) and float the tetra and pyra elements. Smooth the penta elements 5 or more iterations. Now freeze the penta, quad, and tri elements and smooth the pyra and tetra elements at least 5 iterations.

Now go to Edit Mesh > Split Mesh > Split Prisms and enter the desired prism parameters. This will create multiple prism layers from the 1 you extruded.

Now go back to the smoothing tool and smooth the pyra and tetra elements a few more times with all the other elements frozen.
  Reply With Quote

Old   April 24, 2008, 11:10
Default Re: MESH ERROR
Francesco - University of Florence, Italy
Posts: n/a
Thenk you for your guess... now i will try to modify my mesh. The problem was born because after the mesh generation it's impossible to export the mesh like a fluent mesh file.

  Reply With Quote


Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On

Similar Threads
Thread Thread Starter Forum Replies Last Post
Building OpenFOAM1.7.0 from source ata OpenFOAM Installation 46 March 6, 2022 13:21
c++ libraries and solver compiling vaina74 OpenFOAM Installation 13 February 3, 2012 17:43
[swak4Foam] groovyBC: problems compiling: "flex: not found" and "undefined reference to ..." sega OpenFOAM Community Contributions 12 February 17, 2010 09:30
[Netgen] Installation of Netgen in SuSE Linux 92 edvardsenpriv OpenFOAM Meshing & Mesh Conversion 23 January 16, 2009 06:12
Problem with compile the setParabolicInlet ivanyao OpenFOAM Running, Solving & CFD 6 September 5, 2008 20:50

All times are GMT -4. The time now is 16:31.