NASTRAN – Drilling DOF for parabolic shell elements
Question about the behavior of Nastran with regards to the drilling degree of freedom of parabolic shell elements.
I have a model created with 10-node tets and 6-node tri elements. The shell elements are embedded into the solids in order to transmit the rotational degrees of freedom. Using AUTOSPC, I see that the nodes belonging to solid elements appear in the grid-point singularity table for the 4,5,6 DoFs, and nodes for the shells appear for directions that roughly correspond to the drilling degrees of freedom. The shell normals are not necessarily parallel to the coordinate axes.
If I take a flat mesh of parabolic shells (TRIA6) with shell normals pointed exactly in the y-direction, and run groundchecks with autospc=yes, the model will pass all ground checks (through A-SET). The gridpoint singularity table in the .f06 file shows that the 5-direction was constrained (the drilling degree of freedom corresponding the rotations about the Y-axis)
Now, If I take the same mesh and rotate about the x-axis by an arbitrary amount <45 degrees (I chose 10 degrees) so that their normals are “mostly” aligned with the y-direction, but not exactly, the model no longer passes ground checks. It fails in the 5-direction at the N+AUTOSPC-SET which indicates to me that the grounding failure occurs because of improperly assigned SPCs on the drilling degrees of freedom during the AUTOSPC routine.
AUTSOSPC improperly constrains the DoF corresponding to the coordinate axis that is most aligned with the shell normal. Because of this, the model will not pass ground checks (it first fails during the N+AUTOSPC-SET in the 456 directions). I have checked my PSHELL properties, and verified that I have membrane, bending, and coupled membrane-bending properties properly assigned for a full-stiffness plate
element. I have also tried using the MPC option for AUTOSPC, but that similarly did not pass ground checks.
Since PARAM K6ROT only applies to linear shell elements, is there some other way to constrain/stiffen the drilling DoFs for parabolic shells other than AUTOSPC?
Answer – For simple cases (planar faces), you could assign SPCs in a new coordinate system aligned with the shells, or define explicit MPCs that correspond to the true direction of the drilling degree of freedom; however, in a large model with lots of shells with differing normal directions, this may become an unreasonable task as the user would need to create new coordinate systems for every grid point based on the shell normal.
Unfortunately there is no other alternative for it as you are using parabolic shell elements. Instead of that if possible please use linear shell element such as CQUADR,CTRIAR as this elements have a normal rotational (drilling) degrees-of-freedom.