This is my first use of prepromax which looks very promising (but not my first modelling in the FEM field).
The following example is composed of 4 quadratic quads fully integrated under bending conditions:
I can notice that in ccx (see doc), shell elements are in reality “expansed” ans in reality transformed into 3D elements: S8 becomes a C3D20 with 3x3x3=27 integration points, S8R becomes a C3D20R with 2x2x2=8 points of integration and so on
(more time/ressources consuming - i’m also wondering how the connectivity/coincidence is guaranty on the nodes, but it’s not the debate here)
when the stress field is displayed on the 3D expansed elements (default), we get the stresses at both the “upper” face and the “lower” one
when 2D display, i feel the stress field correspond to the middle surface => is it possible to chose either the lower or the upper surface?
Another difficulty: i tried to used rigid body elements connected to a master nodes, but only middle nodes have been linked: what am i missing (see last screenshot)
Anyway, beautifull tool: congratulation for all the works
If OUTPUT=3D, the 1d and 2d elements are stored in their expanded three-dimensional form. In particular, the user has the advantage to see his/her 1d/2d elements with their real thickness dimensions. However, the node numbers are new and do not relate to the node numbers in the input deck. Once selected, this parameter is active in the complete calculation. 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.
So you normally want to avoid 2D output for shells.
This is just a visualization, lines are not created for all nodes. If you check the node set used for the rigid body constraint definition, it should have all the selected nodes.
there’s classical shell element in CalculiX called US3 with default 2D output of top and bottom surface, but analysis type is limited.
Output 2D of continuum shell element can be usefull to extract in-plane or membrane stress. Another purpuse is required for deformed mesh of geometric imperfection in nonlinear buckling analysis. Original nodes and element kept instead of expanded ones.
US3 => linear triangle dedicated to elasticity and isotropic materials.
Ok i can imagine the strategy of Guido Dhondt when using expanded elements:
shell elements in elasticity: 3 integration points in the thickness
hexa/wedge elements = expanded shell = 3 layers
so in elasticity, i can imagine results would remain close (not tested on my side)
nontheless, in plasticity, the number of integration points is increased to 5 for shell elements …
I really admire the works performed by Guido Dhondt and Klaus Wittig for more than 2 decades, but, in my opinion, we should be avare about some limitations … in anyway we’re dealing with prepromax here
it seems to be mentioned in the composite section (section 6.2.14); i do not think it is the case for an (isotropic) material; futhermore, the fig in the S8 section + the log of the ccx file which indicates 27 points of integration (3x3x3) i.e for a single c3D20 let me think we only have 3 Gauss points in the thickness.
it’s still unclear to me how 1D/2D element actually implemented in CalculiX, but several mentioned in documentation many treatments has been done internally, not only doing expansion to 3D solid element.
below an example of 1D beam from documentation, and probably 2D shell element also.
That’s right, for non-composite shell sections, there are only as many integration points as in the case of the solid element to which the shell is expanded. Only for composite sections the number of integration points through the thickness is twice the number of layers.
In Abaqus, one can choose the integration rule (Gauss or Simpson) and number of section points (integration points through the thickness).
This is specific to B32R beam elements with a rectangular cross-section:
In order to avoid hourglassing a 2x5x5 Gauss-Kronrod integration scheme is used for B32R-elements with a rectangular cross section. This scheme contains the classical Gauss scheme with reduced integration as a subset. The integration point numbering is shown in Figure 76. For circular cross sections the regular reduced Gauss scheme is used.
this treatment for eliminated hourglassing of quadratic solid element (C3D20R) of expanded beam (B32R). It maybe applied to quadratic shell element (S8R) also due to similarity, but i’m not known surely.
i can confirm this treatment only applied to quadratic beam element (B32R), number of integration point of solid expansion differs from standard C3D20R. Unfortunately, it’s not yet available for quadratic shell (S8R) even tough sharing similarity in approach. Hopefully that will have the same treatment for quadratic shell element in future version of CalculiX.
