I am new into NX world and I am facing a quite difficult issue.
I would like to import pressure loads (that I have in .nas format) into my model and mesh.
Main problem is I have not done anything like this before (I used to import results from another model as a 'Loads from output' in a previous job using Femap, but never in NX and never from a different software); moreover my model has many parts (shells) and those are quite close in some areas.
I tried using 'from field' load (importing data table from .nas) but, every interpolation method I tried, gave a different and not really reliable load pattern.
Could anyone help me solving this issue?
Are you trying to apply the pressure loads to a selection of element faces or to a selection of polygon faces? Whenever I've set up distributed loads using fields, I've always found that Pre/Post does a very good job of interpolating the loads as long as I apply the field to polygon faces. If I apply the loads to element faces then the accuracy of the interpolation depends upon the consistency of the size of the elements.
I wish I had more specific suggestions for you, but I have limited experience mapping distributed loads onto a FEM and I've never tried to import loads from a .nas file. Hopefully someone in the forum can give you more complete guidance.
Have you tried the Face from Mesh command? It should allow you to create polygon faces from the 2D element faces and then apply the pressure field to the polygon faces.
Creating faces from existing meshes
No, I haven't tried that command.. I hoped that it would have worked on the mesh itself because loads were obtained on a quite similar mesh, so nodes' coordinates should have been quite close to mine.
I would give a try with the surface command (could parts' overlapping create the same problem I have with elements in load interpolation, even with surfaces? Have you ever had anything with more than one part in this kind of analysis?)
It should not matter whether the loads are applied on polygon faces or element faces. In the end, the data written to the solver input deck is in terms of nodes and elements. Polygon geometry is just an additional intermediate step (the exporter will collect nodes/element faces related to a polygon face, then evaluate at those related nodes or element faces).
Ultimately, the field will be evaluated at the element face centroid or at the nodes (depending on the type of load being applied)
Note that, depending on the relative density of the field data and mesh, you may need to try different interpolators to acheive the results you want.
If you are applying forces using a geometry based field (i.e., loads defined based upon X & Y dimensions along the surface) then if you apply that field to polygon faces, Simcenter takes into account the area of the element faces attached to a node to determine the amount of force to apply to the node in the solver input deck. If you apply that field to nodes, then the loads applied are based only upon the X&Y dimensions and do not take into account the area of the element faces attached to the node.
The image below shows the differences in the loads applied at each node when the same field is applied to polygon faces (top figure) or nodes (bottom figure). If the loads are applied to polygon faces, then when the mesh size increases, the amount of force applied to the nodes increases to account for the larger area of the element faces.
I've never imported a distribution of forces from a .nas file but if, after import, those forces in the field are defined based upon coordinates then I would imagine that Simcenter would perform the same way as it does in my example.
Now you are talking about mapping forces, not pressures. Forces are evaluated as you indicated. Equivalent nodal forces are determined and a FORCE card is generated in the input deck. During a solution, their direction is fixed.
My previous post was talking about pressure mapping. There are several methods that can be used here as well (evaluating the field at the face centroid or the nodes; having a single value per face or a single value per node exported, etc.). This results in a PLOAD4 being generated in the input deck. This is a true pressure load and, in nonlinear large displacement analysis, the load direction will update as the underlying face deforms.
All of the simulations I run have multiple polygon bodies in them. You can use a field and apply it to multiple polygon faces from multiple polygon bodies.
I was wondering if you were talking about pressure loads (PLOAD4) and not force loads (FORCE). I've never applied a pressure load so don't know how Simcenter maps those in the input deck.
As usual, the devil is in the details.