Multipoint Constraint Equations for Rigid Body Elements in MSC Nastran 1

[aabaig2022]

Linear Static Analysis Users' Guide of MSC Nastran states that it internally generates MPC equations for all RBEs used in the FE model. Is it possible to view these internally generated MPC equations?

Why do I want to view these MPC equations?

There is a problem solved in the Linear Static Analysis guide with both MPCs and RBEs. I have attached the screenshot for your kind reference. I want to know, when using RBEs, how does MSC Nastran internally generates these equations? For example, in the RBE approach there is no mention of 0.5 unit distance (highlighted in the attached image). How will MSC Nastran determine this when internally generating the MPCs?

Thank you.

 

[dmapguru]

The 0.5 constant is obtained from the relative location of the GRID points. In the image you posted, the diagram in the upper right corner (labelled finite element model) shows GRID points 2 and 3 at a Y distance of 0.5 from GRID point 1; this is the moment arm to multiply by the rotations about the Z axis, as indicated in the first 2 equations.

If you still want to see the coefficients of the equations (which are not output as standard), you will need to use a small DMAP alter to output the RMG matrix generated by the GP4 module. If you look at the module prototype for GP4 (in the DMAP Programmer’s Guide), you will see key datablocks as input to GP4, notably GEOM4 (contains the rigid element), GPDT and BGPDT (GRID point definition tables where the coordinates are available), CSTM to resolve any local coordinate system directions.

DG

 

[aabaig2022]

@dmapguru Thanks for so much for your reply. I will look into DMAP programming.

 

[dmapguru]

If you get stuck, just let me know. You will need a DMAP license to allow the compiler to work.

DG