A common NASTRAN error is SEKRRS. If your model doesn't run properly you should check the *.f06 file for fatal errors. If you see something like this:

^^^ USER   FATAL   MESSAGE 9137 (SEKRRS)   

 ^^^ RUN TERMINATED DUE TO EXCESSIVE PIVOT RATIOS IN MATRIX KLL.

 ^^^ USER ACTION:  CONSTRAIN MECHANISMS WITH SPCI OR SUPORTI ENTRIES OR SPECIFY PARAM,BAILOUT,-1 TO 

 ^^^ CONTINUE THE RUN WITH MECHANISMS.

You are not alone. This is one of the most common errors users experience. It can be frustrating when you do not know what it means or how to fix it, but it is often a simple fix/repair to your model. Though there can be many reasons for it the most common is insufficient constraints. This is typically caused by a few different sources:

1. Inadequate constraints on your model that allows rigid body motion
2. Cracks in your mesh
3. Un-connected mesh
4. Coincident un-equivalenced nodes that should be merged

Many users are tempted to use the PARAM,BAILOUT,-1 option (as suggested in the error text) telling the solver to allow the rigid body motion, however this should be used with extreme caution because it is usually not the intent of the model to allow this. The option once enabled is easy to forget and can cause the model to solve but give the proper results if rigid body motion was not intended to be allowed. The debugging procedure recommended is as follows:

Debug the Mesh:

Perform a normal modes analysis without including any constraints. This should result in, by default, the first 10 modal solutions. The first six modes are the rigid body modes for your mesh, if you have mesh that isn't connected properly you will see more rigid body modes and easily be able to identify the parts that are not properly connected.

Debug the Loads & Constraints:

Only once your mesh is good should you proceed to debug the boundary conditions and loads. First the constraint set should constrain against rigid body motion for your mesh. A free body diagram will help you determine if you have adequate constraints. Depending on your specific geometry and where your constraints are placed the structure should not be able to move or rotate in space if an arbitrary load is placed on the structure.

Once you have adequate constraints your last step is to debug your loads. The most common load issue is non-inclusion in the solver file (*.bdf, *.dat AKA bulk deck). This can easily be checked by reading in your bulk deck into a blank pre-processor file and checking what is read in visually. If your loads are there, and connected to mesh that is constrained as discussed above you should now be good.