I am on SW2009, so I cannot open the file. However, for a sheet metal part, you really should use a shell mesh instead of solid meshing. This thread (see here) discusses the thin versus thick option for shell meshes. As this part appears symmetric, I would also suggest considering using the symmetry option as well, and using a "curvature based mesh" instead of the "standard mesh". Verify the "draft quality mesh" is not checked in the advance tab.
In areas where the part is experiencing high stress, increase the number of elements using mesh control. Unfortunately, adaptive mesh (h-adaptive) options are not available for shell meshing. I suspect the problem you are experiencing with the shell mesh is not applying mesh control (see here for example).
I hope this helps, and Merry Christmas / Happy Hanukkah.
mesh control is set and the part is not symmetric...it appears because I've concentrated stress in the curvature flange, so to remove this stress, I've created this shape, but I would like to return to the first project.
Anyway...when curvature mesh and when standard mesh ?
For this simple sheet metal part or in general sheet metal part..do you suggest shell mesh ?
Do you know the real difference from shell and solid mesh ?
And weld feature how do I have to consider ?
There is another discussion about shell versus solid mesh (see here) that you may find helpful. I posted an image in this link showing an assembly consisting of sheet metal parts. I always use shell mesh for sheet metal, and mixed mesh for combination of sheet metal and solid parts in an assembly. A shell mesh requires less calculations to solve than a solid mesh. I suppose you could use a solid mesh for sheet metal if the element size is dense enough, but the number of degrees of freedom (D.O.F.) used in the calculation would be larger (slower solving time) for the solid.
When I use a split line for the purpose of mesh control, I test both the standard mesh and curvature mesh to see the arrangement of the elements. If the standard mesh elements appear skewed or is not meshing properly, then I use the curvature mesh (see here and here).
Since I do not use weldments frequently, I am not sure about the best practices. Since it is not actually an assembly, I do not know if a mixed mesh can be used. From my training class, the instructor used extruded features to connect the mitre flanges in place of an actual weldment, then solved using a shell mesh. These features where controlled using configurations (see images below). Hope this helps.
In most cases, shell mesh for thin parts is a good way to go. Results are comparable to solid with a lot less processing.
In SW Simulation (COSMOS), all meshes are tet or triangular meshes. This can lead to unnatural stiffness in a shell mesh unless the mesh is parabolic. Setting the mesher to use high quality instead of draft quality will make parabolic elements (6 nodes per triangle) instead of linear (3 nodes per triangle).
As I am using SW2009 (SP5.0), I imported the Parasolid file and used FeatureWorks to rebuild the features for this shell FEA study (see attached file). I did not know the material (galvanized steel ?), or all the boundary conditions (including load force & location), but here is the result using a shell (thin) mesh as shown in the image. The hole sizes may somewhat differ from your SW2010 part model.
For the high stress areas, I used a split line / mesh control for increased mesh density and a curvature based mesh. The solving time was only a few seconds and the number of DOF is approximately 41376. There is also a option to "Save all plots as eDrawings" which I use to share with SW users of earlier versions.
flangia_12-26-2009_SW2009.zip 178.6 KB
Looks like you have had some helpful posts here. A couple of further points may be of interest. I've found that solid meshing can be simpler than shell meshing when you take into account the fiddling around that must be done with defining and solving contacts for a shell mesh.
However, one of the main problems with using a solid mesh on a relatively thin part is that if there is a variation in stress due to bending across the part in section, this is often not evident. The reason is because you need two or three elements across the thickness of the part to show up the variation in stress.