1. I saw there is only spot welding option but i wanted to define continous seam welding. how can i define it? i want to define it on imported model. does i need to used any extra feature for it.
2. while i imported moded as parasolid, i run analysis as solid materail but how can change this materail into desire material type like plate, beam etc.
3. does welded joint and glue feature are same?
4. what is the midsurface model in reality and what its benifit?
• Continuous seam welding: the regular method is to meerge nodes between parts using matching mesh, this way you are assuring displacement continuity between welding parts. For instance, in the following example you have two ways of solving the problem: Shell meshing using CQUAD4 elements & Solid meshing using hexaedral CHEXA elements.
Due to powerful computers, you might consider modelling the actual geometry of the weld. This could be done in basic research but from an industrial point of view it is not practical, because the geometry of weld scatters greatly.
In the case of plate elements the weld is typically not modelled and the finite elements are arranged in the middle of the individual plates. Only if the weld has eccentric weld arrangements is the weld modelled. Examples are shown in the figure below. The main focus must be to take the structure’s change of stiffness into account and if it is greatly influenced by the weld then this must be considered.
If you import in FEMAP a solid model as Parasolid you need to decide the GEOMETRY IDEALIZATION TYPE you want to follow: if meshing with 2-D Shell elements or meshing with 3-D solids, if meshing welds or not.
If you decide to mesh with Shell elements then MIDSURFACE extraction should be performed in FEMAP as part of the job preparation of the geometry for meshing: the thickness of the solid part will be a property of the 2-D shell elements.
Here you are an example of one structure meshed with Shell elements where Fatigue analysis in weld seams is performed using the winLIFE code integrated in FEMAP.
Fatigue damage and utilization ratio results can be obtained and postprocessed back in FEMAP after performing the Fatigue analysis using winLIFE:
If you import a solid model and you want to model the actual geometry of the weld, but the weld is not included, you can do it in FEMAP simple creating geometry, here you are an example:
The weld geometry is created in FEMAP: simply sweep the profile around the seam weld!!.
The FE model is meshed in FEMAP using solid hexaedral elements CHEXA, with excelent quality:
Finally, GLUE connect is different to matching (merge) mesh, but the target aim is the same. Glue is a simple and effective method to join meshes which are dissimilar. It correctly transfers displacement and loads resulting in an accurate strain and stress condition at the interface. The grid points on glued edges and surfaces do not need to be coincident. Glue creates stiff springs or a weld like connection to prevent relative motion in all directions.
What method to use?. It depends if the requirement of the FE analysis: if you are performing a normal modes/eigenvalue analysis using NX NASTRAN (SOL103) then GLUE is perfectly valid, but if you need to perform a Fatigue analysis in seam weld then for local accuracy reasons a matching (merge) mesh is required, forgot at all the glue feature.
Ah!, the last one: advantages of midsurfacing?. Well, I think I have explained the differences previously: shell meshing is great when you are dealing with plate bodies where thickness is very small compared with the other dimensions. If you plan to mesh a steel structure using solid elements, please note you required at minimum two elements in the thickness, then model size will result in millions and millions of nodes & elements, being impractical its solution, OK?.
Thank you very much blas molero for your kind answer
Now i have still question for solid element
i have 4 diffrenet eleme in solid model where
1. plate element with 10 mm thickness
2. square beam 40by40mm with thickness 3mm
3. L-shape beam 40by40 with thickness 3mm
4. circular beam with 40 mm thickness
So i analysis with them as solid element and i got result and as you said there is miliion nodes. is that analysis is incorrect?
As your suggestion mid surface extraction also not a right soloution because i have thick plate. so i decided the 3d-solid element.
My result is mostly to analaysis a stress ,strain and displacement so as your suggestion glue property will also work insist of weld.
There are many ways to model a weld joint. Some are more accurate than others. However, I do not think this is where you should focus your efforts.
The big problem is that you are interested in an area that is typically a singularity (stresses will not converge to a solution as you refine your mesh) unless you model a very small, and arbitrary, radius at the toe or the root (this is generally not practical for real structures).
So, either you are either extracting "far field" stresses (some distance away from the singularity) or using nodal equilibrium forces or element forces to extract a "structural stress". This is true for static or fatigue failure criteria.
You might try to search for information on the "SAE weld challenge".