Hi All, before starting I want to thank all for sharing this beautiful GUI friendly Sowtare for free.
I was trying to simulate basic shell thickness command in Prepomax, I already read the article in shell direction discussion. My question is when i use 2D surfaces to simulate my problem i am having question in my mind that what is the reference point for shell thickneses and its direction.
In the PrePomax the direction of the face is described as Front face and Back Face, Does it give the thickness in the direction of front face or it is the midsurface that calculates both the front and back face? If front so, what about the vertical stiffeneres?
I tried the implement the idea of on way thicknes at 1 and front and back thickness at 2 but, what happens if bottom plate front face is up and vertical stiffener to left side, and flange about up direction. How it calculates the intersection?
Do I need to impose offset or something? Because if i impose offset it will offset in the face direction right?
what must be the correct formulation for this kind of problem, How I can take into account of thicknesses and their directions correctly.
Kind Regards,
Deniz
I also watch the youtube video about the stiffener but only thicknesses are included to show the different thicknesses not the direction..
Yes, offset allows you to use the top or bottom surface instead of midsurface (or even offset the shell further away). It uses the face (and thus also element) normals, but can be inverted by specifying its value with minus sign. This diagram on the FreeCAD wiki explains how it works: https://wiki.freecad.org/FEM_ElementGeometry2D#Properties
2 Likes
Thank you very much, it is a very helpful diagram. But How about the vertical stiffener on a plate, How I can Define correct form?
It looks impossible to shift vertical stiffener to upper position when the normal faces left side?
Does it automuatically shifts vertical stiffenere respect to bottom plate or intersects with it my mind is confused at that point?
Kind Regards,
Deniz
You can just offset the bottom one to avoid the material overlap:
1 Like
How you are able to look at 2D surface as 3D shell element like in the example that you did?
For the complicated geometry how i can manage for example this?
You can see the expanded shell mesh if you run the analysis or use the Check Model option on the Analysis object (that’s what I used here). Just make sure that Output is set to Default or 3D in the Element output definition.
A simple offset (acting only in the normal direction) is not always sufficient to avoid the material overlap. More complex connections will still have it (as well as curved regions). This is normal when using this kind of approximation. It’s usually acceptable, but you can always use solids for the interface itself (and connect them with shells further away via tie constraints or tied contact):
Or even use shell-to-solid submodeling (run the global analysis with shell elements and then make a solid submodel).
However, keep in mind that contact and tie constraints take shell thickness into account, so you can also physically offset the surfaces (move them away from each other) if needed, taking into account their expanded shape:
1 Like
