I have a small model I made. It is two bodies, connected by some CBUSH's, and there are 2 RBE3 elements that are respectively connected to the nodes in each body (so they are averaging the motion of each). I used zero-length RBE2 elements to nodes at the same location as the RBE3 centers. Then, I used 6 MPC equations to constrain a separate GRID point to be the relative motion between the two nodes (one for each DOF) according to 0=-U_out + U_upper - U_lower. I ran a random response analysis (SOL SEMFREQ) and got output PSDs for the z-direction, which is the only direction I excited to make it easier.
I expected the input node and lower RBE3 node to have very similar PSDs (and they did). I also expected the upper RBE3 node and the MPC-constrained node to have similar PSDs. They did not. The MPC-constrained one was 0 at all frequencies. What have I done wrong?
There is no case control command to actually activate the MPC equations. You need to select the constraint set which references the MPC in the "Constraint equation" box on the boundary condition form. The case control will look like this:
CEND TITLE = NX Nastran Modes Analysis Set ECHO = NONE DISPLACEMENT(PLOT) = ALL SPCFORCE(PLOT) = ALL ESE(PLOT) = ALL METHOD = 1 SPC = 1 MPC = 10001 BEGIN BULK
I would also suggest not connecting the entire model to the RBE3's. I would suggest just using the 4 corner nodes of the block to represent the motion of the part. Connecting rigid elements in series like this might not give the results you expect, and for real models that may be large, can degrad performance significantly.