I have a lug and clevis. Lug is modelled using mid surface meshing with QUAD4 elements. Clevis is modelled with tet10 elements. Lugs and clevis are connected with a combination of RBE3 and Beam elements. When a normal modes analysis is run, all the degrees of freedom (of TET10 elements) are failed in the rotational directions. The model did run with out any fatal errors but my f06 file is huge. As the solid elements do no have rotational degrees of freedom, what would be the best method to couple out rotations when using rigid elements?
3-D Solid CHEXA and CTETRA elements (as well as CPENTA & CPYRAM elements, of course!) have only translational degrees of freedom TX, TY & TZ, no rotational DOF are used to define the solid elements. Solid elements contain stiffness only in the translation degrees of freedom at each grid point.
You may either constrain the singular degrees of freedom manually or you can let NX Nastran automatically identify and constrain them for you using the AUTOSPC parameter. Also any combination of the solid elements with elements that can transmit moments require special modeling.
In general, the connection between 3-D solid elements and 1-D CBEAM elements using rigid elements is quite easy:
RBE3 elements are a powerful tool for distributing applied loads and remote mass in a model. Unlike the RBAR and RBE2 elements, the RBE3 doesn’t add additional stiffness to your structure.
If you want to learn more about RBE2 vs RBE3, visit my blog:
Yes, in fact, in models with millions of 3-D Solid HEX/TET elements the file size of the F06 is huge (can be hundred of MBytes): the reason is the PARAM,PRGPST that in recent versions of FEMAP is YES by default. If PARAM,PRGPST is set to NO (default is YES) in the NASTRAN Bulk Data Options, the printout of singularities is suppressed, except when singularities are not going to be removed. This is dangerous, but now you know how to reduce the size of F06 file, OK?.