In either SOL101 or SOL601 I want to get a component to rotate 60 Degrees in order to get the mechanics to lock together.
When I setup the enforced displacement I set Rot Z 60 Degrees.
Trying to solve this the program states that I cant to this as I have to specify more DOF in the enforced displacement as the component is made from a solid mesh.
I think this is very strange as the component as the component cannot be displaced other than by rotation. It is in contact with a surface below, has a cylindrical constraint in its axis (rotation around Z free) and will be locked by a fricktional surface in Z upwards when it starts to rotate.
Why does the program not let me rotate the component?
I have tried different degrees of rotation (1, 5, 60) - the same result.
The solid element formulation only defines translational stiffness terms. In an all solid mesh, there is no rotational stiffness at any grid point, so loads/constraints cannot be applied to DOF 4, 5 or 6. Note that this is true of any standard continuum stiffness element formulation in any finite element solver - it's not particular to NX Nastran.
To be able to apply a rotation, you need to add elements with formulations that provide stiffness in the rotational DOF you want to load/constrain. Typical methods to do this include embedding 1 row of shell elements into the solid mesh, using a RBE2 "spider" element to couple the loaded/constrained grid to several surrounding grids or manually creating a "spider" with legs consisting of CBAR/CBEAM.
Note that 60 degrees is a large rotation, so SOL 101 (linear, small displacement theory) would probably not be appropriate. You can use SOL 106 or 601,106 for a geometric nonlinear analysis. Note that if you use SOL 106, the RBE2 method noted above will not work because the constraints do not update with displacement.