Hi everyone,
I would like to use Prepomax/Calculix to do FEA analysis according to ASME standard, for pressure vessels calculation.
The plan is to use a thick shell model. For ASME stresses classification, it is needed to extract the membrane and bending stresses. I guess they already exist in the shell formulation, but I have pretty much no idea about how to extract them, and maybe (if not too complicated) rearrange them to obtain an image of membrane and bending stresses.
Their formulation is quite simple though. I just need to apply the equations below at each node, and I guess that stresses at mid surface, inner and outer surface are already known when using a thick shell model.
Any idea about how I should/could proceed ?
Thank you in advance.
SĂ©raphin
CalculiX doesn’t have true shell elements, these elements are internally expanded to solids. You can’t obtain top/bottom stresses like in other software, but you can use this setting:
If you set it to 2D, you will essentially remove bending stresses:
If OUTPUT=2D the fields in the expanded elements are averaged to obtain the values in the nodes of the original 1d and 2d elements. In particular, averaging removes the bending stresses in beams and shells.
But you will have output only from the midsurface (or top/bottom surface if you use offset). With OUTPUT=3D, you will get all the stresses.
Actually, there is one true shell element, US3, not supported in PrePoMax, but can be defined using keywords: Support of shell user element (US3)
This element provides the SNEG, SMID and SPOS output variables for the stresses at different locations (bot, mid, top), so maybe you could use that. This element has some significant limitations, though:
The shell formulation is implemented as element US3 in CalculiX and can be used for static and dynamic linear elastic (small deformations) calculations under the consideration of isotropic material properties.
Hi, I made FEA for ASME components and the more easy way is just use Mecway FEA, it has the stress linearization directly available in the GUI.
1 Like
FreeCAD FEM also includes the stress linearization tool, but it has some limitations/flaws and awaits rework: https://wiki.freecad.org/FEM_PostFilterLinearizedStresses
Code Aster + Salome Meca approach: https://www.youtube.com/watch?v=g9Kvv7PYF34
Thank you all for your answers.
I tried a bit to use the US3 user elements but can’t get to any result, probably because of my poor usage of the keywords editor, but I guess it would do the job.
The other options (Mecway and Freecad) seem interesting, but they both use solid models (or do they ?).
Currently, at work, we do it with Castor Concept (a very niche FEA software). It is very practical because you can vizualize the membrane stresses (or bending/total) on the whole shell model just as you would with a VM stress for example. This allows the user to avoid having to select manually the location of the linearization, since it’s done at each done. So, a very practical tool, but the user interface is awful and we have so many bugs…
It might be easier to define it after exporting the .inp file from PrePoMax (since the keyword editor doesn’t allow you to change the existing keywords). Check the CalculiX forum for more details/examples: Missing element US3 - CalculiX (official versions are on www.calculix.de, the official GitHub repository is at https://github.com/Dhondtguido/CalculiX).
Yes, that’s right - you define a path through the solid element layers. But CalculiX’s shells are expanded to solids anyway. Keep in mind that if you use a composite shell section in CalculiX, you will get multiple layers of solid elements (even if they have the same material properties).
