Now I can access it. The first problem I’ve noticed is this: Don't apply concentrated force load to surfaces
However, to check the connections, you should run a frequency step first. Regarding them:
- you should refine the mesh (especially on the welds) and consider using extruded hexahedral mesh wherever possible (then you could switch to linear C3D8R elements)
- you can use the Search Contact Pairs tool to generate tie constraints automatically (just check them and remove the redundant ones e.g. between the plates if not needed due to welds)
- tie constraint should have master surface on the coarser side (the automatic tool doesn’t check that)
- you may need to disable adjustment (to avoid mesh distortion) and increase position tolerance for some tie constraints
Try applying those tips in this file (I started doing it there just to show you the idea, but you should continue with mesh refinement and tie constraint corrections):
Remodeled FEA2 mod.pmx (2.7 MB)
Note that I defeatured the top part to mesh it with hex elements. If you want to keep the subfaces for load application, partition the face in CAD (e.g. FreeCAD can do it easily) instead of making shallow cutouts.