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?
Re: MESH ERROR
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.
Re: MESH ERROR
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.
|All times are GMT -4. The time now is 00:15.|